# Mike's P.M. Research No. 6 Steam Engine



## macardoso

Hi All,

Buddy of mine at work approached me to see if I could help him complete a P.M. Research No. 6 Steam Engine kit that he bought 10 years ago. He used to work as a high school shop teacher and had access to machine tools, however not long after he bought the kit, he was laid off. He had only done a couple of the parts and had probably 95% of the work left to do. Now I get to have all the fun machining the parts, and he gets to keep the finished steam engine. I've been looking for a project so this will be perfect.

Engine Specs:

Bore 1-1/2”
Stroke 2-1/2”
Double Acting
Height: 7-1/2″
Length: 18″
Width: 8″
Flywheel Dia: 6-7/8″
Rating: 1/4 HP






						Steam Engine #6 | PM Research
					






					www.pmmodelengines.com
				




I wanted to start this post to document my progress and ask questions when I get stuck.


----------



## macardoso

I opted to start with an easier part to get started on this project. I used some stock I had on hard since I hadn't yet gotten the stock from my friend.




I have a '94 Enco 12x36 Belt Drive lathe and a G0704 converted CNC mill which I'll be using for these parts. I always clean my benches before I start working. I have a rolling cart that makes a great mobile work station to set up near the lathe or mill.




I started from 3/8" brass stock, first turning the thread diameter and single pointing the 5/16-18 thread. I opted for a 2A thread class.




The first attempt ended in sadness when I accidentally split the 1/4-28 thread. I am threading in a captive segment and then parting off, so I don't have any time to remedy a bad engagement of the threading lever. I was going to press on a new piece of brass (That's why it has been turned down to a stud) and try again, but I opted to just start over.




The single pointed thread (while accurate) had a very poor finish. My lathe had never single pointed nicely without really bad chatter on the flank of the thread. It can take some really heavy cuts normally, so it has something to do with the leadscrew/halfnuts.

The second attempt I single pointed to half depth and finished with a split die. This gave a great finish and the thread over wires was 0.0002" over the center of the tolerance - nice!




Bar was extended and a live center used. The second thread will be cut captive again in the area painted black.




Thread diameter cut, about to start threading the 1/4-28. This went perfectly this time and mic'd over wires at .0004" over the center of the 2A tolerance. After the threading was done I finished the bar to 0.3125 and got within 0.001" over the entire length.




This finish is as-machined using CCGX inserts. Super happy with it.


----------



## macardoso

Next I made 2 Oil cups from the same 3/8" brass bar.




I don't have pictures of it, but the 10-32 thread was first cut with a die and the blank parted off. I then faced, drilled, and tapped the end of the barstock to make a fixture for the second operation.

The oil cup was threaded onto the bar, faced to length, drilled, reamed, chamfered, and finally lightly polished.




Here are the two completed oil cups. They were super easy to make so I may revisit them later to add an aesthetic radius on the sharp edge.




I did scrap one attempt when I accidentally jammed the large drill into the part when moving the tailstock in. It bit into the part and snapped the thread off inside the fixture. I removed it using a #4-40 LH tap.




I am cleaning the parts, packing them in protective tubing, and bagging them up.




I've also started a collection of all the scrap that I'm making  




Not worth writing home about, but I made a simple brass pin which will be hand fitted during assembly of the engine.


----------



## macardoso

Next I started on the piston which requires moderate precision. The kit provides you with a small chunk of 1018 CRS, but I opted to cut it from a larger bar of 41L40. This made fixturing a bit easier too.




Here's my lathe with the 41L40 bar.




I mark all my material like this to prevent a bucket of "Mystery metal".




I don't have pictures from the first operation, but the OD turning was done with a CCMT fine finishing insert to a diameter of 1.4986. I'm pretty sure it is down to 1.4985 now after a bit of polishing.

The grooves were cut with a 0.059" Groove N' Turn insert from Kaiser tool (promo picture below). The inserts are $15 and the tool was $110 (purchased for a paid job), but you can't beat them for quality and performance. I plunged straight into the part and then just fed over to cut the groove. Right on size!




Here is the part after parting. Finish looks better in person (as it always does).







For the second and 3rd operation, I bored and split an aluminum ring. The part was dialed in for axial and radial runout using my Interapid 0.0001" dial test indicator. I called it good enough when I got to about 0.0003" TIR. The trepanning was cut using a brazed carbide boring bar since I didn't have an indexable one this small. The center hole is reamed 0.2500". This operation is repeated on the other side.




All done! Finish is excellent. My lathe imparts a visual swirl pattern when facing (visible in photo). It certainly can't be felt but I'd love to know why that happens. 




Here is a test fit with the teflon sealing rings. They are a firm but really nice fit into the grooves.


----------



## f350ca

Thanks for posting your (his) project. 
Built a PM No 1 a few years ago, was a fun project.
Ran across a set of castings for a Stuart No 4 about a year ago. That turned into an addictive project, couldn't leave it alone.

Greg


----------



## macardoso

That's where I'm at right now. If I really love this once I'm done, I may have to get one for myself. Honestly the idea of not keeping the finished product doesn't really bother me so far.

I can see there is a lot of work that will go into this. I've never started machining a raw casting that didn't have some kind of precision surface, so that will be an adventure. Probably going to be asking for advice on that.


----------



## Lo-Fi

Love it, keep the updates coming!


----------



## macardoso

Finished The Eccentric Hub, a part that turned out to be kinda tricky!




To start, I turned down the barstock of 41L40 do the lip diameter of 1.62". Using my Thinbit grooving tool, I cut the edges of the journal to almost full depth. The first attempt to traverse the groove resulted in breaking the insert ($15 ouch!) and scrapping the part. On the second attempt, I tried using my threading tool to turn the groove and it worked beautifully!




I got the diameter and width within 0.001 and came back with the Thinbit tool to finish the journal floor and walls to size. Journal was 1.4981" and slot width was .502". I'm really happy with that!




The journal was polished with extra fine scotch brite before parting the piece off. The is about 0.0002" of concavity across the journal, probably from polishing. I left a nub of material near the tailstock to help me indicate the part in later.




I made another split ring to hold this part in the 4 Jaw chuck.




Kate felt like hanging out and watching me work. Not sure why she picks the ice cold surface plate as a cozy place to lay down?




To dial in the eccentricity, I first got the part running true both radially and axially within a tenth or two. Then I zeroed the test indicator and backed the cross slide away by 0.250" (verified by the dial indicator). Then I adjusted the jaws of the chuck to throw the part out of center. As I got close, I would rotate the chuck to find the high spot using the DTI, once that read zero, I knew the part was correctly aligned for the eccentric throw. My only gripe is that I had no way to re-verify the axial runout after I dialed in the eccentricity. If I were to do it again, I would leave a much larger diameter nub to indicate on. I think I ended up with about 0.001" of axial runout of the shaft bore to the journal. Would have preferred this to be much less.




The part was faced to final size, and the through hole drilled and bored to a snug sliding fit on a 5/8" shaft. I don't trust reamers to get me on size, so I opted to do it with a boring bar. I think my tailstock needs alignment. The two tone of the steel on aluminum is pretty neat.




The part was flipped in the split ring, indicated for zero axial runout, and faced to final size.




For the final operation (the threaded cross hole), I put the part in the jaws of my mill vise and used a pin and indicator to clock the part so the cross hole was exactly aligned across from the throw of the eccentric. Basically I'd rotate it a tiny bit, find the high spot with the indicator, then rotate it a bit more. Eventually I'd find the maximum high spot which would occur when the cam was perfectly vertical.




The part was centered up using a electronic edge finder. The cylindrical ball allows you to center on symmetrical 3D surfaces which is really handy.




The hole was drilled and tapped 10-24. I was really scared of breaking the tap, but it ended up fine!




4 setups and 8 hours of work went into this part, but it is very accurate and well within tolerance. I sprayed it down with rust preventative and bagged it up!

-Mike


----------



## Chewy

Excellent!!  Please continue updates with your progress. I am interested in building steam engines this summer.  I will be following how you do different steps and the results.  Charles


----------



## macardoso

Finished up one of the packing nuts that I started over the weekend. This part was fairly simple and was a good change to practice some more single pointing.




Didn't get any pictures of the threading, but I basically cut a relief groove behind the thread and took many passes while checking for final dimension within a 2A thread class. Hit it right in the middle. The center bore was reamed, but I got a really garbage finish. Not sure why...




The hex was finished to dimension and gently polished.







In this closeup, you can clearly see the chatter marks on the threads. The tool cuts cleanly, the thread assembles fine, but it just looks weird. I haven't been able to pinpoint why it happens or how to fix it. The tool cuts without those mark when it is used without the leadscrew, but has those marks while threading.  

Center bore is on size, but the finish is pretty poor.




I used this LH ID threading bar to chamfer the front and back corners of the hex.


----------



## ACHiPo

Nice work!


----------



## macardoso

Totally forgot to keep this thread updated. I've made a ton of progress on it and will work on getting photos added as soon as possible.


----------



## Lo-Fi

Yes please!!


----------



## macardoso

I purchased a 3' bar of precision ground 12L14 steel in 5/8" diameter. This stock is straight and round, but soft and easy to machine. I parted off 2 bars which will become part of the crankshaft. They will require later processing to add keyways.




Next I made the valve rod packing nut




The OD was turned from 1/2" hex barstock. The part was drilled, tapped, and reamed thru to 3/16"




I used an internal LH threading bar to chamfer the hex. 




I packed the parts inside expanding plastic mesh to protect them.


----------



## macardoso

Next I started on one of the more complicated pieces, the Frame.




I began with some bench work to remove the flash and seam lines with a file.




The part was then clamped on the milling machine and the feet were cut flat. Care was taken to make sure the bore was parallel to the table and the feet were level.




I left some meat on the casting to allow me to come back and finish them to size after cutting the bore.




I spent about an hour and a half aligning the part on the lathe such that the feet and bore were parallel to the bedways, and the bore was centered. PM Research doesn't give you a ton of extra meat on the castings, so you need to be fairly accurate in the alignment. 




I used a 3/4" boring bar with a few different CCMT inserts to finish the bore to 1.5003-1.5006" which was exactly what I was shooting for. I had about .0002" of taper across the 5" part with about .0002" of bow in the center of the unsupported section of the bore. Not much I can do about that without grinding.




The finish on the bore is very smooth with no chatter. The grainy look is due to the normal tear out of graphite from grey cast iron. Those rough edges were hand filed smooth later on.




The part was placed back on the mill and I used a DTI to carefully shim the part such that the bore was parallel to the bed of the machine. 




Checking the machined height on the machine.




Made a big oops by hitting the "Page Down" key while facing the part by hand. This jogged the Z axis into the part. I carefully removed a thin web of material from the middle to create "feet" for this Frame. It was a mistake but I made it look OK.




Finally the feet were drilled. The holes are perfectly placed, however the casting itself is crooked hence why the holes aren't centered on all the feet.




All that is left is drilling the bolt hole pattern for mounting it to the cylinder head and tapping a hole in the top for a drip oiler.


----------



## macardoso

The next part I tackled was the Base. It is a fairly large casting and requires facing the top, bottom, and drilling/tapping 16 holes.







I first clamped the part upside down. I used a 1/2" HSS roughing endmill to face the bottom of the part, moving whichever clamp was in my way. The change in clamping pressure around the perimeter created a few steps in the face but they won't be visible when this is assembled. Not sure how to do it better. After about 1/3 of the way around the part, my spindle load meter started to climb, the finish got worse, and the cut got louder. I stopped to find my endmill was worn to a smooth corner. It must really not like the scale right at the surface of the casting. I switched to a carbide roughing endmill from Hanita and has no further issues.




I then flipped the part and skimmed the top faces for full cleanup. This actually took the part underside on the height, but was the preference of my friend who owns the kit.

Right before I started on this side, my CNC computer had a glitch and wouldn't respond to the mouse or keyboard (touchscreen was fine). I had to fully reimage the PC including setting up Mach 4 again. That sucked and chewed up 2 weeks of shop time. But everything is running fine again.





After taking 2 weeks off from working on this, I wasn't in my flow, wasn't paying attention to the print, and made a big oops. The mounting pads shown below were for 10-24 screws, but I pre-drilled them #7. With permission from my buddy I will have to modify the plans to use 1/4-20 bolts here for the pillow blocks instead.

The process of indicating this part to be straight on the table without any precision surface to reference, and to center the holes on the various bosses took many hours of fiddling with the indicator. I probably spend twice the time on setup as I do actually cutting.




Here is the mating part with the intended screw (left) and the 1/4-20 screw (right). It will look and function fine, but I'm mad at myself for not paying attention.




Here are the pads completed. I also drilled the 4 mounting ears at the bottom.




Kate needed to do a final QC.

There was also several hours of bench work to remove the flash from the edges of the casting.




-Mike


----------



## macardoso

Next I worked on the valve head (outboard exhaust) using the included piece of 1018 CRS.




OP1 was to finish the 0.62" diameter and the predrill, then part off to length




Then the part was filpped in a 4 jaw chuck, indicated within .0002" of runout, and the precision diameter was turned and the part made to length.




I didn't own the 1/8" NPT tap when I started this part so I tried to tap it later. Held in in a chuck while tapping but it slipped and really mucked up the precision diameter. I could probably salvage it, but it was easy enough to make that I'll just make another and tap it before parting off. Kinda bummed about that.

I'm really enjoying working on the lathe, so I'm saving a lot of the drilling of the bolt holes for later.


----------



## macardoso

Next I did the Inboard Valve Head. I don't have a picture of the print for this one, but it was very similar to the other valve head except it has a 3/8-24 thread on one end with a 3/16" reamed hole through, instead of the 0.62" diameter with a 1/8" NPT through.

I turned the thread diameter and single point threaded away from the chuck. I feel I'm getting better at this and can get within a 2A tolerance very comfortably now, usually within a half thou of nominal.




I checked the thread over wires and also against the packing nut that it mates with. The fit is excellent but it cannot bottom out due to the tap runout inside the packing nut. I may retap it deeper or relieve the threads inside.




I parted off the chunk I needed and saved the off-cut to use as a fixture for OP2. I tapped it 3/8-24 then faced it to clean it up.




Here was my single point threaded first operation.




The part was then threaded onto the fixture nub and indicated true to the OD and the machined face.




This allowed me to easily access all of the features for OP2.




And the part is finished except for the bolt holes. To be done at a later date.


----------



## macardoso

Next I started on the valve. The critical diameters are .623-.624 and they are used to seal the steam in the valve cylinder. The stock is only .6245 to begin with, so I needed to be very accurate in centering the part in the 4 jaw. Unfortunately I couldn't get both diameters within .0005" TIR for whatever reason (cheap 4 jaw?) so I dialed in the runout near the end of the valve and cut that diameter as well as the middle of the dogbone. I used some new tools including a RH and LH VCMT tool which made grooving the dogbone very easy. The center is drilled and reamed to partial depth as .5010" and drilled and reamed through .1875". The sealing diameters were cut to .6238"

I re-indicated closer to the chuck to finish the second diameter, adjusting it by only a few tenths.




The part was cut off and flipped to finish the second side. I held the valve in an aluminum split ring fixture to prevent scarring on the part from the jaws.




Here is the nearly finished valve. There are two cross holes that need to be done on the mill which I haven't done yet.


----------



## macardoso

Next I worked on the Inboard Cylinder Head. It is a casting that is cleaned up on all sides.





I held onto the little nub of material to finish all the cylinder side features in one setup. A CCMT insert with a large corner radius was used to rough in the casting and one with a small radius was used to finish it.




There was not enough material on the casting to finish this diameter to spec, however it is non-functional, so my buddy and I decided to reduce it to full cleanup.







After this picture I drilled and tapped the 1/2-20 hole for the packing nut.

Here is that part fit to the Frame. There is no play between the bore and the pilot diameter




Shown with the packing nut installed in the frame. This seals the piston rod for the return stroke.


----------



## macardoso

I'm working on the Cylinder now which I bored the 1.5" hole to 1.5005" (exactly what I was shooting for) and the fit to the piston is beautiful. I'm struggling with the Valve cylinder (machined into the same piece parallel to the main cylinder). It is .6250" and 3.4" long. At 7:1 extension ratio (1/2" bar) it is too long to bore so I settled on using a reamer. I've done some test pieces in 1018 mild steel and have gotten holes with cruddy surface finishes and diameters between .6255 and .6258 which is too loose and sloppy for the .6235" valve. With lots of oil it is moderately air tight but with a normal amount of oil for running it is leaky.

I've had hit and miss results with reaming and it is possibly due to the quality of the reamer. The two I have tried are some I inherited. Good name brands and moderately sharp.

I'm wondering if I will just have better luck with machining the casting? Maybe a new reamer? Maybe an undersize reamer (.6240")? Would love any tips for getting this right. I checked my tailstock a month or two ago and found it to be well centered (within .0003") and true to the spindle (within .0004" over 4" ).

My goal is a nice air tight sliding fit (maybe .0005"-.0010" clearance?)

EDIT: Worst case I can make a new valve to fit the finished bore, but the surface finish is really bad too, so at a minimum I need to improve that.


----------



## bakrch

1018 is incredibly difficult to get a finish on. Can't say I remember reaming this material (my guess is that engineers know to avoid this in the design phase), but turning/boring usually requires a bazillion RPM's and cermet tooling to get a passable finish. Are you able to test in a different material? I can probably send something to you, but I surely do not have cast iron. F22, F91, 416, 316, 17-4 PH, 440C are all available for me to send.

Personally, I would ream undersize and hone it to finish if possible. It is impossible to know how that reamer is going to cut in your particular setup unless you have a spare pc to work with to cut under the same conditions.

edit: on second thought, boring it with a solid carbide 1/2" bar may chatter a little bit, but honing that away would produce a straighter hole.


----------



## ErichKeane

FYI, I love this thread!  It has encouraged me to get my own PM Research kit!  I ordered the No 3 Steam Engine last night!

Assuming I can get it finished, my idea is to see if I can attach it to a tea-light powered steam boiler


----------



## macardoso

bakrch said:


> 1018 is incredibly difficult to get a finish on. Can't say I remember reaming this material (my guess is that engineers know to avoid this in the design phase), but turning/boring usually requires a bazillion RPM's and cermet tooling to get a passable finish. Are you able to test in a different material? I can probably send something to you, but I surely do not have cast iron. F22, F91, 416, 316, 17-4 PH, 440C are all available for me to send.
> 
> Personally, I would ream undersize and hone it to finish if possible. It is impossible to know how that reamer is going to cut in your particular setup unless you have a spare pc to work with to cut under the same conditions.
> 
> edit: on second thought, boring it with a solid carbide 1/2" bar may chatter a little bit, but honing that away would produce a straighter hole.



OK well that makes me feel a lot better. I got really frustrated trying to get this right last night. Here are some pictures from my test part. Photographing surface finishes is hard but maybe these will help show my difficulty. It looks like a bad boring job rather than precision reaming.







Another difficulty is getting a 3% pre-ream drill for .625". I don't have anything close to a .608" drill so I was boring it (with a TON of chatter) to around there and then reaming. My closest drill is 9/16" (.563").

I'd definitely be game to try another material as a test piece. I don't know what the closest thing to cast iron would be. I'd be happy to pay for a small cut of whatever you think is good. (Let's skip the stainless, I hate stainless  )

Found a new .6240" reamer on ebay for $28. I'd have to reduce the shank, but I think that would work for me. A carbide boring bar is an option, but I just don't see being able to get a great finish. How would you hone the bore? Ball Hone? Link Here




ErichKeane said:


> FYI, I love this thread! It has encouraged me to get my own PM Research kit! I ordered the No 3 Steam Engine last night!
> 
> Assuming I can get it finished, my idea is to see if I can attach it to a tea-light powered steam boiler



Congrats!

I'm having an absolute blast with this. Be warned, they are a lot of work. I've been counting my hours and I'm looking at around 50 hours setup and machining so far and I don't know if I'm halfway yet. That doesn't count cleaning the workshop, researching, or recording my progress here.

I'm also a bit of a perfectionist, so if I get a dimension out of tolerance and I have replacement material (so everything but the castings) I will start over. Probably not necessary to get a working engine but I want it to be perfect for my buddy.


----------



## ErichKeane

3/4" Cast Iron is about $1/inch on speedy metals: https://www.speedymetals.com/pc-4274-8388-34-rd-gray-cast-iron-class-40.aspx

I'm assuming on the size   However, for about $20 shipped, you could get a dozen tries


----------



## Lo-Fi

Meehanite is lovely to work with, mess aside. No hard spots or inclusions and great machinability. I've made a load of bearing journals, gears and suchlike out of it.


----------



## bakrch

macardoso said:


> OK well that makes me feel a lot better. I got really frustrated trying to get this right last night. Here are some pictures from my test part. Photographing surface finishes is hard but maybe these will help show my difficulty. It looks like a bad boring job rather than precision reaming.
> 
> View attachment 317416
> 
> 
> View attachment 317417
> 
> 
> Another difficulty is getting a 3% pre-ream drill for .625". I don't have anything close to a .608" drill so I was boring it (with a TON of chatter) to around there and then reaming. My closest drill is 9/16" (.563").
> 
> I'd definitely be game to try another material as a test piece. I don't know what the closest thing to cast iron would be. I'd be happy to pay for a small cut of whatever you think is good. (Let's skip the stainless, I hate stainless  )
> 
> Found a new .6240" reamer on ebay for $28. I'd have to reduce the shank, but I think that would work for me. A carbide boring bar is an option, but I just don't see being able to get a great finish. How would you hone the bore? Ball Hone? Link Here



I will look for some 416. Sure it's stainless, but it machines very easy believe it or not. It finishes pretty dull, but doesn't tear like 1018 would.  The above cast iron solution is also a pretty good idea.  Up to you, the offer still stands. (no charge for this, these are in the scrap bin anyway)

Yes, a drill hone is what I was thinking ... assuming you can deal with the bottom of the bore, like maybe putting a lead on the part that slides in to account for the unreachable areas (if it even matters).


----------



## macardoso

bakrch said:


> I will look for some 416. Sure it's stainless, but it machines very easy believe it or not. It finishes pretty dull, but doesn't tear like 1018 would. The above cast iron solution is also a pretty good idea. Up to you, the offer still stands. (no charge for this, these are in the scrap bin anyway)
> 
> Yes, a drill hone is what I was thinking ... assuming you can deal with the bottom of the bore, like maybe putting a lead on the part that slides in to account for the unreachable areas (if it even matters).



I'd really appreciate that if you wouldn't mind. Might also look into the Cast Iron.

This is actually a through bore. There are valve heads on each side, so the machining is surprisingly easy given what it is.


----------



## bakrch

macardoso said:


> I'd really appreciate that if you wouldn't mind. Might also look into the Cast Iron.
> 
> This is actually a through bore. There are valve heads on each side, so the machining is surprisingly easy given what it is.



Okay, no luck with 416 but I did snag a pc of 440C (1.5" dia @ close to 4" length).  Still not going to be too bad to machine it.


----------



## macardoso

bakrch said:


> Okay, no luck with 416 but I did snag a pc of 440C (1.5" dia @ close to 4" length). Still not going to be too bad to machine it.



You are awesome, thanks.


----------



## macardoso

This past weekend I had some time to work on the steam engine some more. I've been doing the harder casting parts lately, so I decided to work on some of the easier parts on the lathe.

I started with the Lower Valve Rod, which was a simple rod with a 10-24 thread on one end and a cross drilled hole on the other end. When complete, the part will be bent to shape to fit the final engine. 

I started with the 10-24 thread using a die. I have a full set of "Little Giant Screw Plate" taps and dies. They look like high quality tools, however after I ran the 10-24 die over the part, it did not cut 24 threads per inch. It was closer to 21 and very sloppy. Not sure what that was all about. Fortunately I also had a "normal" split die for a 10-24 which ended up cutting perfect threads.




All of the dies have two movable jaws that have screws coming in from the outside which adjust the size of the cut thread. Pretty interesting. 




I parted the bar to length but did not yet drill the cross hole.

Next I squared up some brass stock on the lathe for what will become the Upper and Lower Linkages. I was able to get the cut to length within 5 tenths.




I used a 4 jaw self centering chuck held in a 3 jaw self centering chuck to cut these pieces from the short piece of barstock provided in the kit.




I cleaned them up with 600 grit sandpaper and bagged them for later use.




My buddy bought a hardened and ground shoulder bolt to use instead of machining the wrist pin, however it measured significantly undersize on the diameter so I decided to go ahead and make the wrist pin. I've never seen a shoulder bolt be the wrong size?




I've been having a lot of issues with the carriage travel on my lathe being very inaccurate and not repeatable. I'm wondering if there is a damaged gear or loose pin in the apron, or perhaps the rack and pinion is messed up. To cut this part accurately, I set of a 1" dial indicator on a flexible arm.




I turned the thread major diameter for a 10-24 thread and used a split die to cut it. The stock is CRS hex provided with the kit.




I used a VCGT insert to undercut the thread on the end and finish the outside diameter. I turned it to .3125" with .0001" of taper along the .875" length. This is larger than the kit called for, but I only have a .3135" reamer so the fit will match what the kit called for.




I parted the part to length, but paused before fully cutting it off to use a LH internal thread bar to put a 60 degree chamfer on both sides of the hex.




Finally, I reamed an aluminum tube in place in the chuck to .3135" and placed the bolt in there. Tightening the chuck to crush the tube held the part with near zero runout and no marring of the precision surface so I could finish the head of the bolt.


----------



## hman

macardoso said:


> My buddy bought a hardened and ground shoulder bolt to use instead of machining the wrist pin, however it measured significantly undersize on the diameter so I decided to go ahead and make the wrist pin. I've never seen a shoulder bolt be the wrong size?


Wellll ... Chinese persons do tend (on average) to be of smaller stature than westerners.  So it's understandable that their shoulders might also be narrower.  Recall the occasional references to the size of Chinese horses on the forum


----------



## savarin

Awesome work, cant wait for the final steam up.
Thanks for showing this makes me want to do something similar.


----------



## macardoso

So I haven't written here in a while because I've mostly been posting about completed parts and lately I've done a ton of parts half way. Over the weekend and last night I finished 6 different parts. I'll do a big dump of those now. I've also done most of the work on the main cylinder including the piston bore and valve bore. It just needs to have the bolt patterns drilled.

Here we go with the updates:

To prepare for the pile of parts I want to run on the mill, I loaded 24 tools into CNC tool holders and preset them all on the bench with my 8" height gage.




This is what my tool table looks like.




And the completed pile of tool holders. This is pretty much all I have. The values were keyed into Mach 4.




The radiused outside was completed with a quick 10 second CNC program with the No. 3 1/4" endmill. The relief pockets were cut using the MPG jogging functions on the CNC as were the drilled holes.




The second part requires a mating slot to be cut through the middle. I opted for a dynamic slot milling operation using a 1/8" endmill. With a light finish pass on each wall I got a great fit on the first try. I did goof and the finish pass clipped the corners of the slot when plunging and retracting. This was just a couple of thou and I blended them into a chamfer with a piece of emery cloth.




Here was the No. 6 1/8" endmill




The completed clevis.




Here the pieces are mated. I failed to get a good picture of the completed parts but they had a 3/16" hole drilled on the ends and a 1/16" cross hole drilled for a roll pin.

After chatting with my buddy, we decided to go off print and use a 45 degree chamfer cutter to remove the razor edge on the part with one tab. It is cosmetic only.


----------



## macardoso

Next I continued on with the inboard head, drilling the bolt hole circle. Something odd to note is the holes are not evenly spaced. This is to allow the bolts to pass into the frame without hitting some webs on the casting.




I had to remove the jaws from my vise to fit the part. It was supported on parallels and gripped with brass shims. 







Holes cut like butter. I was moving the parallels around to avoid drilling them and to support the part.




Here is the complete part. I ordered a 1/2-20 bottoming tap to finish the center hole deeper.




And fitted in place on the cylinder (sneak peak!)


----------



## macardoso

Remember this little guy? This is the inboard valve head. I finished the lathe work a while ago but needed to do the bolt hole pattern.




I made a super quick (read TOO quick) fixture by tapping a 3/8-24 hole into a piece of scrap aluminum and threading the part onto it as firmly as possible.




The holes were spotted and drilled to the print. I got a little aggressive with the first hole and the part spun slightly. Fortunately the drill bent and didn't break or mess up the part other than a very minor amount of bell mouth on one hole. This was acceptable and I was able to finish the part after holding it down better and drilling more slowly.




Complete. You may also notice the kitchen peeler got my finger


----------



## macardoso

These shafts were next on my list to check off the list.




My friend wanted to keep one shaft a little extra long to allow him to attach additional hardware. The shaft and keyway were lengthened by 1".

The part was indicated flat within 5 tenths then centered with the electronic edge finder.

I used the Mach 4 multiline MDI to write a quick G-code program to slot the keyway in 3 passes. The fit was perfect on the key.




A couple of quick wipes with an Arkansas stone removed the razor edge. 




I repeated this process for the second shaft.


----------



## macardoso

Easy one done last night. 

I had finished OP1 and OP2 on this valve a while ago. I set it up in the vise on parallels and indicated it flat. Then used the electronic edge finder to locate the center of the stub end.

I drilled the cross port with a 3/16" drill followed by a 1/4" endmill. I was cutting a cross hole pretty close to the diameter of the part, so I wanted to use the end mill to keep it on diameter and straight. It came out great.




I then added the 1/16" cross hole for a roll pin. I used a 1/8" endmill to spot face the hole before spotting. The witness mark from that operation is still on the part.




And finished! It took me a long time to really understand how this valve works. The cross hole allows the inboard side of the cylinder to exhaust to atmosphere through the middle of the valve to the ouboard side of the valve cylinder.


----------



## BGHansen

macardoso said:


> The next part I tackled was the Base. It is a fairly large casting and requires facing the top, bottom, and drilling/tapping 16 holes.
> 
> View attachment 317223
> 
> 
> View attachment 317216
> 
> 
> I first clamped the part upside down. I used a 1/2" HSS roughing endmill to face the bottom of the part, moving whichever clamp was in my way. The change in clamping pressure around the perimeter created a few steps in the face but they won't be visible when this is assembled. Not sure how to do it better. After about 1/3 of the way around the part, my spindle load meter started to climb, the finish got worse, and the cut got louder. I stopped to find my endmill was worn to a smooth corner. It must really not like the scale right at the surface of the casting. I switched to a carbide roughing endmill from Hanita and has no further issues.
> 
> View attachment 317222
> 
> 
> I then flipped the part and skimmed the top faces for full cleanup. This actually took the part underside on the height, but was the preference of my friend who owns the kit.
> 
> Right before I started on this side, my CNC computer had a glitch and wouldn't respond to the mouse or keyboard (touchscreen was fine). I had to fully reimage the PC including setting up Mach 4 again. That sucked and chewed up 2 weeks of shop time. But everything is running fine again.
> 
> 
> View attachment 317226
> 
> 
> After taking 2 weeks off from working on this, I wasn't in my flow, wasn't paying attention to the print, and made a big oops. The mounting pads shown below were for 10-24 screws, but I pre-drilled them #7. With permission from my buddy I will have to modify the plans to use 1/4-20 bolts here for the pillow blocks instead.
> 
> The process of indicating this part to be straight on the table without any precision surface to reference, and to center the holes on the various bosses took many hours of fiddling with the indicator. I probably spend twice the time on setup as I do actually cutting.
> 
> View attachment 317227
> 
> 
> Here is the mating part with the intended screw (left) and the 1/4-20 screw (right). It will look and function fine, but I'm mad at myself for not paying attention.
> 
> View attachment 317228
> 
> 
> Here are the pads completed. I also drilled the 4 mounting ears at the bottom.
> 
> View attachment 317232
> 
> 
> Kate needed to do a final QC.
> 
> There was also several hours of bench work to remove the flash from the edges of the casting.
> 
> View attachment 317234
> 
> 
> -Mike


Many die makers in our tool room at work say, "the sign of a good machinist is how well they can hide their F-ups". Great work and saves.

Bruce


----------



## macardoso

I took a little hiatus from this project as I picked up an industrial robot and I've been working on getting that running. Here are some updates on the project as I start back into it.

Here the the inboard head. This seals the main cylinder from the outside.



The component starts as a casting with a remnant of the casting gate hanging from the side.




I rough machined the back of the component to establish a datum.




Next I turned and CNC drilled/tapped an aluminum fixture ring to use on the next operation.




The bolt hole circle was drilled and spotfaces were added under the screw heads at my buddy's request.




I bolted it to the fixture and used my 4 jaw to get the ring shaped boss in the center of the part running fairly true. The OD was turned to size. 




Using some brass shim stock, I finished the back side features.




And here is the finished component! Ready to be painted.


----------



## macardoso

Here is the frame if you guys remember it. It is nearly done with the exception of the bolt hole circle on the mounting face and the oiler port on the top.




And the associated print. Since the head and the cylinder are nearly done, I wanted to get these bolt holes drilled so I could start mating the parts together.




Here is my fixture setup.




I have a big problem that whenever I walk away from machining for a while, I make a ton of mistakes as I get back into the rhythm. I should never start with really important non-replaceable parts. Here I just drilled the spot holes for the bolt hole circle. A smart machinist would have double checked their measurements, but nope! Not me!  




And here are the holes drilled 7/32. This was the exact moment I realized I screwed up. The print is a touch confusing and leads you to believe the holes are equally spaced on the bolt hole circle. Unfortunately the are not and the holes on the left and right side of the image below need to be spaced closer together. This is to avoid getting too close to the casting walls below this feature. Since this part cannot be remade, I have to repair it.




Here was the spot on the print where I made my mistake. 2.312 B.C. does not mean equally spaced. The 1.000 measurement controls the spacing. Unfortunately the correct hole position overlaps the drilled hole position by 50%.




My solution was to purchase cast iron bar stock and turn stitching pins out of it. The incorrect holes are tapped 1/4-28 as it is pretty close in minor diameter to the drilled hole size, but not much larger in major diameter (as to not weaken the casting). 




Here are some practice stitching pins. I was making these quickly and using the lathe DRO Sub-Datum Memory to allow me to change tools and directly read out pitch diameter. I made 2 scrap pins, 2 good pins, and I have 2 more to make. These will be glued in place with Loctite Green and machined flush. Then the holes will be drilled again, with part of the hole machining away some of these pins. The finished repair should be quite strong, and hopefully not too visually obvious.


----------



## hman

Mike -
This thread and your SCARA thread showed up right next to each other in my "watched treads" list.  All I can say is WOW ... Your projects span the gamut from steam engines to SCARA robots!!  

Now all you need to do is build a generator.  Then you can use the steam engine to power the generator to supply electrizicals for the robot to stoke the boiler.


----------



## macardoso

hman said:


> Mike -
> This thread and your SCARA thread showed up right next to each other in my "watched treads" list.  All I can say is WOW ... Your projects span the gamut from steam engines to SCARA robots!!
> 
> Now all you need to do is build a generator.  Then you can use the steam engine to power the generator to supply electrizicals for the robot to stoke the boiler.



I think I might have too many hobbies lol.


----------



## macardoso

Finished all the stitching pins last night. Two of them are 0.56" long and two are 1.38" long. I turned and threaded them in one operation and hit the middle of the 2A tolerance. The DRO made this fairly easy, but I found the threading less easy to trust the DRO numbers, probably due to the higher deflection and cutting forces.




The 1/4-28 tap I had could not thread the full depth for the 1.38" pin, so I used carbide inserts to turn the tap into a reduced shank tap. The steel was very hard, but machined nicely with carbide. Probably was cutting a bit fast and the chips were coming off deep blue.




I tapped the back holes full depth. I think I should have left the reduced shank right at the minor diameter of the thread. The tap seemed to want to walk a little once it was deep in the hole.




Here are the stitching pins installed. The shorter ones in front can be threaded in all the way with finger pressure. The ones in the rear get tight at 50-75% of full depth. I think there are two problems... First I dropped the pins and I think there might be some very tiny dings on the threads. Nothing obvious, but a magnifying glass might help. Second, I am worried either the drilled hole or the thread are crooked (or both). The pins are not at all flexible so they bind. 

I will try to run the tap in and out of the hole to try to get the fit better. Alternatively I can add wrench flats to the pins and insert them with additional torque beyond finger tight. They will be glued in place with bearing retaining compound when installed for real.


----------



## macardoso

The stitching pins are installed. Tried a couples things to get the longer ones to fit better, but I just ended up slitting the face with a hacksaw and using a flat head screw driver to drive them in. They all seated to the proper depth so there is no step or divot on the bottom face of the flange.

Loctite 620 was applied to 3 of the 4 screws before installation. I was running the longer pins in and out of the threaded holes to loosen them up, but I got the back left long stitching pin stuck and cracked the head off of it trying to remove it. It is very secure, but I may drill the hole to half depth and add some loctite. It should wick into the crevices in the thread. I am not worried about it coming loose even without the added Loctite.




I am waiting the 24 hours for the glue to cure before facing them close to the original surface and machining the holes. The surface will be lapped to blend the pins into the surface after machining. Hopefully they will be mostly invisible.


----------



## macardoso

Repair is complete!

The Loctite 609 set overnight and I drilled out the holes with a carbide drill. The HSS drill really wanted to walk so I subbed in the carbide. Cut beautifully. Prior to drilling, the stitching pins were machined within a thou and a half of the flange surface.




All that is left is to lap the surface of the stitching pins flat with the flange face and drill the oiler hole on the spine of the frame near the top edge of this picture. I am waiting on my buddy to pick out his oiler so I can match the thread.




Here are two shots of the backside of the flange showing the repair. You can see how close the old holes were to the casting surface which prevented installation of the screw from this side.







I am very pleased with the outcome. This part is pretty much finished until my buddy picks out that oiler. On to the next (easier) part 

Couldn't get a good picture of it, but there is a really cool zig-zag pattern down the wall of the hole where the thread was machined away.


----------



## tq60

You may consider filling the holes with solder.

Flux and low heat and a mess but it will fill in the holes and color will be close enough if leaving bare metal.

If painting Bondo will do.

Sent from my SAMSUNG-SM-G930A using Tapatalk


----------



## Boswell

Nice Save


----------



## macardoso

tq60 said:


> You may consider filling the holes with solder.
> 
> Flux and low heat and a mess but it will fill in the holes and color will be close enough if leaving bare metal.
> 
> If painting Bondo will do.
> 
> Sent from my SAMSUNG-SM-G930A using Tapatalk



Didn't think of that! I'd be concerned about the structural integrity of the repair under load. This isn't anything crazy, but the flange does support the weight of the entire cylinder assembly plus the pneumatic force applied when the cylinder is in the return stroke position. I also expect this part to heat up quite a bit, perhaps as much as 200*F in continuous operation. The Loctite 609 is temperature stable and will retain 75% of full strength at 100*C - although I am not relying on the Loctite for mechanical stability, but rather the thread engagement.

This part will we painted at some point, not sure if my buddy will use bondo or just gloss paint over the rough casting.


----------



## RWanke

Really got my interest up on this. I am looking at PM Researches #3 steam engine kit. I am wondering if the machining on this kit can be done with only a SB 9C lathe and a drill press. I don't have a mill.


----------



## ErichKeane

I did a #3, I think you'd be hard pressed to do it without a mill. There are a few surfaces that need to be milled flat/square that would be not possible without a mill or a really large lathe.


----------



## macardoso

RWanke said:


> Really got my interest up on this. I am looking at PM Researches #3 steam engine kit. I am wondering if the machining on this kit can be done with only a SB 9C lathe and a drill press. I don't have a mill.


I’m not as familiar with the #3, but I could see you making do with a drill press if it were quite stout and you invested in a compound table. Obviously far from ideal, but if you were really gentle with it, and were capable of high quality bench work to finish it up, then you could probably be successful.  
It would be a fun project either way!


----------



## RWanke

My drill press is a Craftsman that I bought around the mid to late 70s (belt drive, 12 speed maybe). I have tried to spot mill a little piece once before using the drill chuck and the chuck kept coming out of the spindle (morse taper if memory serves me). I don't think it's stout enough to do any type of mill work.


----------



## hman

Back in '16 I found a vintage Craftsman drill press at a local Habitat for Humanity shop, "motor no worky," for $25.  I repaired/refurbished it and eventually sold it to a friend.  The really interesting thing about his drill press was the fact that there's a clamp ring above the chuck that holds it in place against side forces.  The original maual mentions router bits.  I kinda wondered if it could also be used for minor milling.



Here's a close-up of the chuck and clamp ring.


----------



## Manual Mac

RWanke go ahead & order the PM No3.
While by no means simple, it’s MUCH easier than this one.
As Eric said you will have some problems without a mill.
But if you have a 4jaw chuck & some endmills you can put in the chuck with MT holder, or even a 3jaw chuck, give it a try.
A milling attachment or some way to hold the base square while u machine it is a must though.
But part of the reason we do these things is to be creative, no?
Macardoso, I an enjoying your build, thanks for sharing.
I have that same Greenfield Little Giant tap & die set, those 2 piece dies are indeed interesting. There is even instructions on how to sharpen them.


----------



## RWanke

Not wanting to hijack this thread and send it in another direction I have done some very small milling on my SB lathe by holding the part in a tool holder and an end mill in the 4 jaw or a collet. I don't have a milling adapter setup for my lathe and might have to do some serious thinking on how to hold a large object on the cross slide to mill. I am assuming the mill work that needs to be done on the No.3 is on the base???? Anyone that has built one of these please feel free to chime in. I may give PM a call tomorrow and ask some questions. Thanks all.


----------



## RWanke

This is from PM's description on their site.

...." With a 2-1/4 inch flywheel and an overall length of 6 inches, this kit will make a great project for the machinist with a small lathe. The casting kit is available with either aluminum castings, or bronze & iron castings."....


----------



## Manual Mac

What I meant was put endmills in MT #2or 3 endmill holders in spindle or 3 jaw chuck if you do not have holders. My bad.
The 4 jaw I used for boring cylinder & facing & irregular shapes, could have done the base with it also, but the mill was much easier.
I also have SB9C.
I am not finished with the PM No 3 bi yet, my 1st casting kit.
Gonna order the PM No 5 next.
Very enjoyable hobby, eh?


----------



## RWanke

I have faced quite a few irregular shapes on my lathe with the 4 jaw. I just didn't know if the base would fit or not. What all has to be milled on the base?


----------



## Manual Mac

I think we’re hijacking this thread.
I am certainly no expert, but send me a PM & I’ll share what little I know.


----------



## Manual Mac

Macardoso, any progress on your No.6 build lately?


----------



## macardoso

Ugh  No, I have this on the back burner. Wife warned me that starting a second project at the same time was not going to work. I bought an industrial robot back in May and have been working to get it running again. It is a blast, but have not gotten much machining done otherwise.









						Mike's SCARA Robot
					

Hi All,  Some of you may have seen me write about how much I am interested in industrial robotics. I've been looking for an old robot to play with for 3-4 years now and one just happened to pop up!    Many people are familiar with the 6 axis articulated robots that are often shown in factories...




					www.hobby-machinist.com
				




I am through most of the larger components and the stuff that is left does not look too bad to do. I think the next step is finishing the cylinder casting by drilling and tapping all of the little holes that mount components.


----------



## macardoso

Well @Manual Mac, you got my interest going on this project again! I normally only write a post when I finish a part, but I've been so slow at this I might as well catch up on where things are.

Previously, I did a lot of work on the main cylinder. It is nearly done with the exception of the mounting bolt circles. I need to do these but I'm a bit nervous to do it since I already have so much time invested in it.

This is the cylinder casting. It requires two faces, two precision spaced and sized bores, bolt circle holes tapped on two sides, steam port hole cross drilled and tapped, and insulation plate mounting holes drilled on the periphery. The #5-40 tap is going to be a bit tricky to find.







The first operation was to dial the part in using the 4 jaw to center the large bore and align the angle of the part. This is the most time consuming part I have found when working with castings. This flat face becomes the part datum.




Once a datum face was established, the part was bored to a precision fit to the piston. This was done using a 3/4" steel indexable boring bar.




Here is the air tight fit. The piston slides easily on a thin film of oil inside the bore, but is pretty tight once the teflon packing is added. I think I need thinner teflon.




Here is the bore finish. I have a bore hone which will be used to lightly cross hatch the surface for better oil bearing. The rough slot on the left is a steam port in the casting.




As mentioned earlier in the forum, I was having a really hard time figuring out how to cut the valve cylinder, which runs parallel to this bore. It is .625" diameter hole, 4 inches long and must be an air tight sliding fit to the steam valve with a light coat of oil. I ended up buying an undersized reamer 0.624 and machining the end to fit my drill chuck. Thanks to @bakrch, I had some 440C stainless to practice machining on and was able to get the fit and finish I needed. The second bore was again painstakingly aligned using a tenths indicator to be centered on the casting, parallel to the main bore to 0.0005"/4" and within the published center to center distance within 0.0007"

Here is the reamer with the reduced shank. Surprisingly to me, the shank is very soft steel.




Practice bore in 440C Stainless.




Offset chuck boring operation.




Here I was measuring the throw of the chuck as I adjusted it. Timing marks were scribed into the chuck jaws and the part to make sure it did not rotate in the chuck during adjsutments.







Once I was confident in the setup (center to center measured as 1.9997"), I drilled, bored, and reamed the hole to finish size.







And here is the final fit of the steam valve. If the valve didn't have a chamfer, you likely wouldn't be able to see the edge between the two parts. The valve slides in the bore with little friction once lightly oiled. Honing this cylinder would be nice, but I don't have a tool to do it.




This is where the cylinder sits today. I need to drill the bolt circle holes and tap them and do the steam valve drill and thread. After the bolt circle debacle on the frame, I am a bit nervous to do this one.

More to come


----------



## macardoso

Started two days ago on what I thought would be an easy part to ease back into this project, but I am concerned I might have picked one of the hardest!

Enter the crosshead!




In this steam engine the crosshead (#12) rides inside the "frame" (#2) to support the piston inside the cylinder. It is linked to the piston using the piston rod (#19) traveling through the inboard head (#3) and the packing nut (#45). The cross head cycles down the length of the frame with every stroke of the piston and serves as the pivot and attachment point for the connecting rod (#11). It has oil passages to collect oil from the oil cup (#44) and disperse it to the sliding surfaces and the pivot bore.




The crosshead comes as one casting, connected to the eccentric arm. These are separated with a hacksaw and substantial bench work was done to clean up the flash.




The part was indicated true on the lathe and the back surface was faced and the internal holes drilled and tapped. I also added my first "apprentice mark" to the lathe jaws  . I was trying to turn the OD and snuck the tool into the bevel near the tips of the jaws. What I didn't see or account for was the other jaws being closer to center and not having the clearance of the bevel at the tip. I am really mad at myself, but it isn't the end of the world. Maybe I can find a set of replacement jaws.

So anyways this part is tricky because it has a number of precision features but nothing to reference. This face and the axis of the pitch diameter of the thread become the datum for all subsequent measurements. I turned down part of the OD to a non-finish diameter to allow me to verify the part is running concentrically in future operations.




OD finishing will be done on this fixture which has been drilled, faced and tapped in-situ to guarantee best accuracy. a 5/16 bolt was loctited in place and faced off to become a mounting stud.




Before finishing the OD, the connecting rod pivot bore and spot faces should be machined. A 3/8" shoulder bolt with a 5/16" thread is tightly installed in the thread and seated against the face. This allows me to accurately indicate the part for angular alignment in the Y and Z axes as well as determine the X, Y, and Z coordinates of the datum. Roll (rotation about the X axis) is not important in this setup and is set by standing the rough cast surface on parallels. My Interapid 0.0001" DTI was used to align everything within 0.0002" over 2"

A CMM thread locator would have been more accurate, but the shoulder bolt should do. In addition, these CMM locators are crazy expensive!









						TRU-POS™ - Tapped Hole Location Gages - STRAIGHT or TAPERED - (Inch) | Judge Tool & Gage
					

Shop TRU-POS™ - Tapped Hole Location Gages - STRAIGHT or TAPERED - (Inch) from Judge Tool &amp Gage, trusted by the world's leading manufacturers, engineers, & designers.



					www.judgetool.com
				







An electronic edge finder was then used to locate the center axis of the shoulder bolt and the datum face.




The reamed hole was predrilled to 95%.




Due to tool holding inaccuracies, the reamer initially had 0.0030" of runout. 20 minutes of careful indicator work and tapping with a lead weight centered the reamer within 0.0003" TIR. John Saunders of NYCCNC taught me this trick!




I didn't have a tool to cut the 7/8" diameter spotface, so I wrote a quick CNC program to mill the pocket with a 1/4" endmill.




And here is where I got to. This whole process needs to be repeated on the second side with the addition of carefully indicating the part in roll to make sure the spotface on the second side is parallel to the first. Then the 2 cross drilled oil holes need to be added, and finally the part can be OD turned for a precision running fit to the frame.


----------



## Manual Mac

I’m really enjoying your build, thanks for bringing us along.


----------



## macardoso

Manual Mac said:


> I’m really enjoying your build, thanks for bringing us along.


Thanks for giving me a kick in the you know what to get started again! Will be switching back and forth between this and programming the robot in the coming weeks/months.


----------



## macardoso

Finished the cross head!

The alignment of the second spot face to the first was very tricky and ended up not being perfect. Some of my techniques worked great while others did not. The first thing to do was align the part rotationally in the vise in all 3 axes. The roll of the part along the X axis was controlled by placing a gage block against the freshly machined surface.




The pitch and yaw about the Y and Z axes were controlled with a cradle I built which pushed against the shoulder bolt. I could indicate the top and sides of the shoulder bolt using my tenths indicator and adjust the screws pressing against the shoulder bolt to align the part. All in all, I got these within 0.0002"/2".







XY center was indicated off the reamed connecting rod pin bore and Z was taken off the top of the center of the shoulder bolt.

The CNC program was run again, first at half depth to measure the web thickness and again a full depth adjusting for error in Z positioning




All said and done, the web thickness measured 0.3751" in the center (nice!) and had 0.0001" of taper front to back, but a really bad 0.0100" of taper side to side. The part ended up not wanting to sit flat on the gage block and was rolled along X for the final machining. This shouldn't cause problems in operation but I was bummed about it. If I were to do it again, I could have indicated the walls of the bore along the Z axis with my DTI and I would have seen the bore was slightly crooked. 




Oil holes were drilled through the part after setting it up similarly to before using a 3/32 drill.




The final feature is a hole at a 60 degree angle from the side which vents air to allow the oil to flow. The part was held in a small Sherline tool makers vise with a 30 60 90 block underneath to set the angle. 




The dowel pin in this setup is critical to ensure the rough cast surface it is resting against did not twist the part in the vise. The part center was edge found from the machined OD and the X position was aligned visually from a scribe line on the part




Drill depth was determined by some basic math off the various features and trig to account for the angle. Would have been easier to just listen for the drill to break through to the center.




The part was mounted on the lathe fixture and indicated true to the previously machined OD and spot faces. OD turning was very quick using a CCGX insert to give the final finishing passes. OD was machined to 1.4990" and the bore of the frame is 1.4998". The fit is so perfect and a light film of way oil allows the parts to slide silently over each other. I bet the fit will loosen as the parts wear in initially and the prominences are rubbed down.


----------



## macardoso

Felt like taking stock of where I am at currently. Here is a picture of a real life exploded parts diagram of the engine (minus screws and missing parts).




Here is a list of machined parts and my status:

Crank Disc (Qty. 2): Partially machined by my buddy, incomplete
Cross Head: *Done (8.5 hours)*
Crank Pin: Incomplete
Lower Valve Head: *Done (2 hours)*
Piston Rod Packing Nut: *Done (1.5 Hours)*
Lower Linkage: *Done (2.25 Hours)*
Upper Linkage: *Done (2.25 Hours)*
Eccentric Hub: *Done (8 Hours, 1 Scrap)*
Wrist Pin Bolt and Nut: *Done (1 Hour)*
Valve Head: Incomplete: Incomplete (1.25 Hours, 1 Scrapped)
Valve Rod Packing Nut: *Done (1 Hour, 1 Scrap)*
Oil Cup (Qty. 2): *Done (1.75 Hours, 1 Scrap)*
Piston: *Done (5 Hours)*
Lower Valve Rod: Done pending final fit (0.5 Hours)
Pillow Block Cap (Qty. 2): Incomplete
Eccentric and Cap: Incomplete
Upper Valve Rod: Done pending final fit (0.5 Hours)
Valve: *Done (3 Hours)*
Crankshaft - Short: *Done (0.75 Hours)*
Crankshaft - Long: *Done (0.75 Hours)*
Piston Rod: *Done (4.5 Hours, 1 Scrap)*
Pillow Block (Qty. 2): Incomplete
Rod and Rod Cap: Incomplete (0.5 hours)
Base: *Done (5.5 Hours)*
Flywheel: *Done (1 Hour) *Buddy did this one, I just skimmed it true.
Frame: Done pending drip oiler selection (10 Hours including repair)
Cylinder: In Process, mounting holes needed (5.75 Hours)
Inboard Head: *Done (3.5 Hours)*
Head: *Done (1.5 Hours)

Recorded hours to date: 72.25 Hours *(probably close to 90 including cleaning, bench work, and planning)
*Estimated Completion: 60%*

And some close ups:

This is the cylinder detail. The piston is sandwiched between the two heads and connects to the crosshead with the piston rod (far right)




Here you can see all the details of the valve linkage.




Here is the crosshead, connecting rod, and frame.




Here are the crankshaft components. This is the most incomplete section of the engine.




Base and flywheel.




Raw stock plus bronze bearings not in the kit for the bearing blocks.




I want to focus on the components needed to start assembling this up on the base. Finishing the cylinder and getting the bearings done will be the next things for me to focus on.

To be continued...


----------



## macardoso

Finished the crank pin last night.

The part started from 12L14 centerless ground barstock.

Since the OD of the part is the nominal dimension of the stock, it had to be indicated in very carefully.




I then skimmed the entire surface to clean up. OD of the part ended up 0.6235", well within tolerance.




The first press fit stub was turned to 0.3765" on a target dimension of 0.376" +0.0005 -0.0000.




To maximize concentricity, all features (other than remove the parting nub) were completed in one setup. I have a LH VCMT insert tool which allows me to do this kind of work. I utilized the DRO Sub-Datum Memory (SDM) as tool offsets to switch between the LH and RH tools. 




I used plunge roughing to start the cut in the middle of the workpiece. I turned the collar to 0.118" on a 0.120" +0.000 -0.002 calculated tolerance. For some reason, my ability to accurately turn dimensions in the Z axis are limited to about 0.001-0.002 while my ability to hold diameter tolerances if I try is 0.0001-0.0002".

The critical running diameter of the pin was finished on the right half to 0.4986" on a 0.499 +0.000 -0.001 tolerance. 




I then finished the left side of the groove with the RH tool to the exact same 0.4986" as the right half. There is absolutely zero blend line between the two. Also the phone camera makes the surface finish look way worse than in real life which is weird.

I turned the other press fit stub the same way I did the center groove, hitting 0.3765". There is a call for a press fit lead of 0.002" off the diameter over 0.060" on each press fit stub. Doing some trig calculates a 0.955 degree angle. This was dialed in on the compound (rounding to 1.0 degrees) and the length of the taper was determined against a scribe line visually. Both sides were cut at the same time. 

I started the parting operation, but waited to go to full depth so I could chamfer the back corner.

A light 45 degree chamfer was made on all corners and finished the parting off.




Finally the part was rechucked in a crush ring fixture, reamed to 0.6240. The part was brought close to true and the parting nub was machined flush to the face. 




Here is the final part. 




Total time was 2 hours. 

As an aside, I don't know how I lived without my Interapid tenths indicator before. It has enabled me to do so much more accurate work.

I think my biggest limit to accuracy is my chuck. While I can dial in the runout to 0.0001", there is a parallelism issue somewhere and the part will sit crooked by about 0.0001-2" over 2". Doesn't seem like much but it is the limit on my work holding accuracy.


----------



## BGHansen

macardoso said:


> To maximize concentricity, all features (other than remove the parting nub) were completed in one setup. I have a LH VCMT insert tool which allows me to do this kind of work. I utilized the DRO Sub-Datum Memory (SDM) as tool offsets to switch between the LH and RH tools.


Nice work as usual; space shuttle attention to details.  I'm going to have to read my DRO manual for the sub-datums; great idea on the tool positions.  Pretty sure mine is one of the Chinese-generics with 200 sub-datums.

Bruce


----------



## macardoso

BGHansen said:


> Nice work as usual; space shuttle attention to details.  I'm going to have to read my DRO manual for the sub-datums; great idea on the tool positions.  Pretty sure mine is one of the Chinese-generics with 200 sub-datums.
> 
> Bruce



Yup, mine is the same. Basically, if you've used a CNC before, it is the same as entering G54, G55, etc. You can zero in each SDM and it doesn't affect the other SDMs. You can use them in a lot of different ways, but on my lathe, I use one for each tool on the job. Zero out the tool as usual, then if you come back to that tool, enter the SDM number and you're right where you left off, no remeasuring needed.


----------



## macardoso

OK, bearing blocks are done. Boy were these more work than expected, about 18 hours in total for the pair. Let me show you the journey.

I started with a 1/2" carbide roughing endmill (Kyocera) to clean up some of the casting remnants from the gate. 




The pair of blocks (and attached caps) were laid relatively flat using a digital level from Shars.




In hind sight I should have done them one at a time, but it worked out OK. My poor mill flexes all over the place when doing this heavier roughing.




The bearings were then clamped to my tooling plate and faced to height. I used a height gage to measure them in-situ.




I also kissed the oil cup bung in that same setup. From there the parts were hacksawed apart and we get two rough bearing blocks.




I opted to lightly finish each side so I had some reference surfaces to clamp in the vise. I also cleaned up the sides of the caps in the same manner. It was extremely non-trivial to decide how much material to remove from each side so the cast features ended up in the center of the caps. I got it pretty good, but I would have approached it a bit differently if I were to do it again.




The oil cup bung was drilled and tapped to the center of the feature, while the bolt holes were centered on the block. These features were 0.005" and 0.007" out of alignment on the two caps respectively. There is no hard requirement for their alignment and it is not visually apparent.




Here is following finishing both caps. A 3/8" diameter spotface is added to each bolt hole so the mounting screws sit against a flat surface.




From here on out, the bearings were machined with their caps firmly bolted on. Each cap was stamped across the parting line to help match them up after being separated. An extra long 3/8" HSS endmill was used to finish both faces in one setup to the specified 1.31" dimension. Since the caps weren't centered perfectly to the casting, these faces ended up not centered to the lower casting either by about 0.005". The mounting holes were also shifted so it shouldn't affect assembly.




The mounting holes are drilled and spotfaced as well. There is also a 1/8" hole through the middle of the lower block, not part of the plans. This will allow a retaining pin to be added which will prevent rotation of the bronze bearing relative to the housing.




This post is getting long so I will follow up with more details.


----------



## macardoso

In the next part, I machine the bore of the bearing blocks.

Out of some scrap aluminum, I drilled and tapped the bolt hole pattern for the lower bearing block.




It was rotated 90 degrees and indicated true in both yaw and pitch within 0.0002" over the surface. The block measurably bowed under the vise clamping force (caused problems later). 




The bearing block was bolted on with a mill fixture used to back up the part and resist cutting forces. Roll about the X axis was indicated within 0.0002" over the length of the machined block.




The block was drilled to 0.500" and then bored to 0.7522" in 0.020" increments. This was an incredibly tedious process.




Thankfully, I used the MDI on the CNC to automate the fine feed and retract.




The fit was supposed to be a 0.0005" interference fit to the bronze bearing, but that ended up being a bit heavy. The bearing really isn't very round or even. It had variations of almost a thou which messed with the fit I was going for. I ended up hand reaming it to an awesome fit to the shaft. Super free with almost zero wiggle in the shaft.




Here is where the problems hit. Since the shaft is such a close fit to the bore, any misalignment would cause binding. I could get the shaft through both bores but when they were bolted down, the shaft was locked tight between them. An inspection later would reveal that one bearing block had the bore out of parallel by 0.0002" over the 1.31" width of the block, and the other was 0.0016". The blocks were mismatched in height by 0.0004". The main issue was the out of parallelism of the one bore to the base by a thou and a half. Multiply this by the 2-3 bearing block widths between the bearings and you got a shaft misalignment of nearly 5 thou. 




How will I fix this? Stay tuned!


----------



## macardoso

Bearing blocks part 3...

I needed a way to correct for the out of parallelism of the bore to the base of the block and to match the height of each block. I figured I would try to scrape them in, because why not?

*DISCLAIMER: I am not an expert scraper. I am not trying to teach anyone how to scape. I do not claim to do it the right way. I am doing this for a hobby. I learned what I know on YouTube. Apparently this needs to be said on this site *

Here is my measuring setup. The granite plate is a grade B, flat within 2um (0.00008"). The flex arm (not ideal, but it is all I have) is holding an Interapid 312B-3 0.0001" DTI with the tip at approximately 12 degrees to the surface giving a true reading. The granite was cleaned with alcohol and allowed to come to room temperature. My spotting dye is High Spot Blue.




My technique is to manually lift the indicator tip, slide the part under and ease the tip onto the part. The part is kept in good contact with the plate and swept to find the lowest point (center of the bore). Both sides of both parts were measured and the lowest one zeroed out the indicator.




I first scraped for good bearing contact as the milled surface was poor. In all these pictures, my bluing is very heavy. This was often done for the camera as the thin bluing was almost impossible to see.




I was using a file with the tip ground to a negative rake with a wide radius. After 2-3 passes, I am starting to break up the mill ridges. I am working at 45 degree angles relative to the part and rotating my scraping 90 degrees each pass.




Once the surfaces were in decent bearing, I could evaluate the geometry. One block was 0.0004" high of zero on one side and 0.0006" high on the other. The other block was 0.0000" on one side (arbitrary) and 0.0013" high on the other. I focused on this crooked one first.




This was done by selectively removing high points from the higher side. I mentally divided the part into 4 bars across the short width. The whole surface got one pass, then 3/4 of the surface of 2 passes, 1/2 got 3 passes and the final quarter got 4 passes. I would correct about 0.0001" of angular error per pass. I would continually check the part for hinging to determine if I was developing a twist or bow as I worked. On the first part, it stayed pretty flat the whole time. After 15 passes or so, I was able to remove all the angular error from the part, with both sides of the bore measuring within 1/4 graduation of the indicator of eachother.




The process was repeated for the second part, First to correct for angular error and then to start bringing the height down. During this process, I noticed the part would hinge directly on its center leading me to believe I had developed a bow to the part. Some scraping on the center only corrected the hinging so it occured at the 2/3 point (centered on the width) opposite where I was pushing it.




Once the blocks were within a tenth of eachother, I went back to the first and ground a smaller file. Using extremely light bluing, I tried to increase the bearing contact. It was pretty easy to identify the burnished locations and mark those with a Sharpie to scrape. The smaller file gave me great control and allowed minimal material removal. After 10 passes of this I was bearing at 30 points per square inch or so.




I used the first block as a reference and scraped the second within 1/2 graduation (0.00005") on the indicator relative to the first. I got the bores on each block even side to side within 1/4 graduation (0.000025)". It was extremely frustrating to take measurements at this level as any dust on the plate would throw the measurements all over the place. Also simply holding the part for a minute or two would cause it to grow by nearly a tenth. My final measurements were taken with gloves on and after an hour of letting the parts come to room temperature. My measurements are for reference only since my indicator was last calibrated 11 years ago and my surface plate has a flatness limit of 0.00008", but man was I excited to be able to control the removal of material to this level.




Remounting the blocks yielded a shaft that spun freely in the bearings. I thought I needed to scrape the base as well, but this was good enough.

View attachment 63382109301__80CC3441-46D8-4D91-939F-AE8C3EC93BB1.MOV


EDIT: No oil in the bearings yet in this video, just showing how easily it spins.

So there went 18 hours of my free time (4 of which were scraping)! Getting closer.

Mike


----------



## macardoso

Had a bit more progress since the last update that I'd like to share.

I focused on the crankshaft next. Remember that this is a 5 piece press-fit assembly (two shafts, two discs, and the offset pin). My buddy got a start on one of the discs which I lightly cleaned up




The second disc was cut to match the first. I had to make the OD slightly undersized from the print to get them to match. The CCMT insert worked great for this heavily interrupted cut. The bore was reamed to 0.624" 




I had to take some time to think of how I wanted to cut the offset pin bore such that each disc had the exact same throw and the webs in the castings were aligned. Any error in the throw of the cranks (relative to eachother) would create a misalignment of the end shafts and they would bind in the bearings.

To accomplish this, I hand punched and drilled a tiny hole in the middle of each of the webs visually.




I then turned and sanded in a 0.6238" arbor that was a tight sliding fit to the bore of the discs. Using a tiny drill bit shank to align the holes, I super glued the discs back to back. 







The super glue firmly held the parts together for the remainder of the machining operations. I set this up in the mill. Unfortunately I did not have any Vee blocks that were big enough to hold the part, yet small enough to fit in the vise (this was a problem later on). I added a hold down clamp to make a hard stop I could push the part against. I cut off a section of the arbor to use as a pin to indicate the bore. 




I first indicated at the base of the pin to find center of the bore, then used a sharp tipped chamfer tool to visually clock the part such that the webbing would be centered on the to-be-drilled hole. I did not yet take any care to accurately align the part to the machine since any effort there would be lost when I loosened the vise to clock the part.




Next, using a tenths indicator, I swept the pin up and down to measure the angular alignment of the part in the vise and tap it into true with a lead tapper. This was time consuming and took about an hour. At the end of the day, I got it within 0.0001" over the roughly 1.2" length of the pin. Once it was aligned, I found center again.




Out of concern that the part might move when machining it, I gently placed a strap clamp on top, tightened to finger tight. This was a huge mistake I would learn later.




The hole was rough drilled




Then I threw in a under sized reamer to cut the precision .3115" bore. When I first mounted the reamer, it had 0.009" runout. Using a tenths indicator, I was able to tap the tool into runout <0.0005". I figure that the flexibility of the tool shank will allow the tool to center up once it hits the drilled hole. 




Unfortunately, once I removed the part from the vise, I could see something was off. The hole wasn't right. I setup a measurement cradle on the surface plate, using the center bore as a datum and measured the hole was crooked by 0.002" in the radial direction and 0.008" in the tangent direction. I suspect between the addition of the hold down clamp, the drilling, and the reaming, the part must have shifted in the vise. 




This amount of misalignment was not tolerable and would cause issues with the center shaft alignment once the assembly was pressed together.

It needs to be corrected... To be continued.


----------



## macardoso

OK, now to correct the parts.

I opted for a new work holding method of a 3.5" 4 jaw scroll chuck clamping the bottom boss. Again, I setup the part with the tight fitting dowel and clocked the part using the tenths indicator. Once it was darn close, I indicated the vertical of the pin and tapped the setup to have about 0.0001" over 1.2" of angular misaignment.




Once the part was sitting true, I indicated the existing location of the small bore and verified the throw of the crank was accurate and within specification using a bit of trig.




The hole was colored with steel blue and fine bored only to full cleanup.




Once done, I setup the measurement cradle on my surface plate a verified the hole was parallel to the bore within 0.0002" in both directions 

The new bore (now slightly oversize from the print was measured with telescoping and small hole bore gages. I really hate small hole bore gages and don't trust them under 0.001. I trust my telescoping gage skills within 0.0002".

A new crank pin was turned identically to before except with larger ends to match the oversized holes.




The parts were cleaned of blue and oil then heated over open flame for about 10 minutes to break the super glue bond. It was super strong. Yes I know our stove deserves some TLC. I cook a lot!




Using the arbor pin, I slowly pressed the parts together on my mill vise. I removed it several times to inspect on the surface plate to verify they were going together straight. All good!







The shaft ends were pressed together on the lathe. The part was held in the 4 jaw, while the shaft was in a big drill chuck in the tailstock. An aluminum plug was placed between the discs with the exact size of the gap to prevent the assembly from collapsing under the pressure.




The reamed hole was a bit light of a press, so Loctite 609 was added to strengthen the bond.




And Done!




The shaft is a great fit between the bearings and it spins very smoothly. A bit of run-in will likely make it even better.




Here is a short clip of the flywheel and crank shaft spinning in the bearings with a light coat of Vactra #2 way oil for lubrication.

View attachment 63545291795__FF3B9F80-9106-42EB-A14A-FB3DEB7E4B18.MOV


----------



## macardoso

The crankshaft is going to be my next major part to work on since it will let me cycle the cylinder by rotating the crankshaft. 

The casting was extremely rough (the worst of all of the ones in this kit) and they two mold halves were not lined up well at all. I spent quite a few exhausting hours draw filing and sanding to get this clean enough to work on. 

I plan to leave most of this casting rough after machining the features, so I'd like it to be relatively attractive.










I jumped back to the cylinder casting to get the bolt holes mounted. The casting was held in the vise against a hard stop and clocked so the bores are in line along the X axis. I got it within a thou. The hole patterns are different on each side and I was very careful to drill the holes correctly lest I repeat my mistakes on the frame.




The holes around the big bore are tapped 10-24 while the holes around the valve bore are tapped 5-40. I centered on each bore before drilling each bolt hole pattern so the pattern was perfectly centered. I did clock the part extremely close, but it is more important to center the pattern on the bore rather than getting the center to center distance perfect.




All drilled and tapped. I lightly stoned the surface with a hard Arkansas stone to remove the burr around the tapped holes and keep the surface flat.




The cool thing now is the bolt holes allow me to assemble a big chunk of the hot end of the engine. Here is the frame, head, cylinder, outboard head, cross head, wrist pin, piston rod, piston rod packing nut, piston, valve, inboard valve head, and valve packing nut. I had zero assembly issues.







Here is the engine as it stands! 







I made up some gaskets with computer paper, and the piston holds air pretty darn well. It needs better gaskets than oiled paper but I'm very happy. 

Major components remaining:

Connecting Rod
Eccentric Ring
Outboard Valve Head
Cylinder (drill/tap steam inlet, drain bungs)
Bearing Sleeve (turn to length, add oil holes)
Frame (drill and tap for oil cup)


----------



## macardoso

Here is a list of machined parts and my status:

Crank Disc (Qty. 2): *Done (4.5 hours)*
Cross Head: *Done (8.5 hours)*
Crank Pin: *Done (4 hours, 1 Scrap)*
Lower Valve Head: *Done (2 hours)*
Piston Rod Packing Nut: *Done (1.5 Hours)*
Lower Linkage: *Done (2.25 Hours)*
Upper Linkage: *Done (2.25 Hours)*
Eccentric Hub: *Done (8 Hours, 1 Scrap)*
Wrist Pin Bolt and Nut: *Done (1 Hour)*
Outboard Valve Head: Incomplete (1.25 Hours, 1 Scrapped)
Valve Rod Packing Nut: *Done (1 Hour, 1 Scrap)*
Oil Cup (Qty. 2): *Done (1.75 Hours, 1 Scrap)*
Piston: *Done (5 Hours)*
Lower Valve Rod: Done pending final fit (0.5 Hours)
Pillow Block & Cap (Qty. 2): *Done (17.5 Hours)*
Valve Eccentric Ring and Cap: Incomplete
Upper Valve Rod: Done pending final fit (0.5 Hours)
Valve: *Done (3 Hours)*
Crankshaft - Short: *Done (0.75 Hours)*
Crankshaft - Long: *Done (0.75 Hours)*
Piston Rod: *Done (4.5 Hours, 1 Scrap)*
Connecting Rod and Rod Cap: Incomplete (2.5 hours)
Base: *Done (5.5 Hours)*
Flywheel: Buddy did this one, I just skimmed it true. *Done (1 Hour) *
Frame: Done pending drip oiler selection (10 Hours including repair)
Cylinder: In Process, steam port and drain port needed (8.25 Hours)
Inboard Head: *Done (3.5 Hours)*
Head: *Done (1.5 Hours)


Recorded hours to date: 102.75 Hours *(probably close to 115 including cleaning, bench work, and planning)
*Estimated Completion: 80%*


----------



## Boswell

A steam engine is on my bucket list, thanks to your detailed build notes including the time and effort log, I have a great idea of what I will be getting into when I decide to move forward on this.


----------



## macardoso

Boswell said:


> A steam engine is on my bucket list, thanks to your detailed build notes including the time and effort log, I have a great idea of what I will be getting into when I decide to move forward on this.


I'm having a blast with it. Honestly I don't care about the hour count, it is all for fun. 

The No. 6 is tied for the biggest steam engine they make. This is fun for me for sure. Only limitation is that is uses a LOT of steam/compressed air, so you need to have a good compressor to run it. Mine may not be able to keep up continuously.

The smaller engines look like less work, but have a ton of tiny parts. Gas hit and miss engines are the next level up and they seems to have a massive jump in complexity and difficulty. I have been follow an Edwards #5 radial engine on here that is super impressive.

I've learned more about machining doing this engine than all of my projects before it combined. Seriously


----------



## ErichKeane

macardoso said:


> I'm having a blast with it. Honestly I don't care about the hour count, it is all for fun.
> 
> The No. 6 is tied for the biggest steam engine they make. This is fun for me for sure. Only limitation is that is uses a LOT of steam/compressed air, so you need to have a good compressor to run it. Mine may not be able to keep up continuously.
> 
> The smaller engines look like less work, but have a ton of tiny parts. Gas hit and miss engines are the next level up and they seems to have a massive jump in complexity and difficulty. I have been follow an Edwards #5 radial engine on here that is super impressive.
> 
> I've learned more about machining doing this engine than all of my projects before it combined. Seriously


I did a PM#3 and had a similar feeling on it!  I thought it was a lot of fun and pushed me quite a bit!  The small parts of the #3 ended up being on a bit fiddly for me, so I kind of wish I'd done one of the bigger engines.

I DID do a hit-miss engine after that, but never got it running :/  It again had some very small parts (and I ended up scrapping about 60% of my tries as a result), and for some reason I just couldn't get it working.


----------



## macardoso

ErichKeane said:


> I did a PM#3 and had a similar feeling on it!  I thought it was a lot of fun and pushed me quite a bit!  The small parts of the #3 ended up being on a bit fiddly for me, so I kind of wish I'd done one of the bigger engines.
> 
> I DID do a hit-miss engine after that, but never got it running :/  It again had some very small parts (and I ended up scrapping about 60% of my tries as a result), and for some reason I just couldn't get it working.



Bummer, that really sucks. Any idea why it didn't run?


----------



## ErichKeane

macardoso said:


> Bummer, that really sucks. Any idea why it didn't run?


No real idea... I had all the necessary components (Air, Fuel, Spark, Compresson) and spent a bunch of time trying to get it to run, but nothing worked.  I eventually gave up on it.

I SUSPECT it might be the carb, which was so small and fiddly that making it was really difficult.  Otherwise, everything else was pretty much on spot.  I had considered mailing/gifting it to anyone on the forum who wanted to make an attempt at getting it running, but I ended up just tossing it on a shelf in my garage.


----------



## brino

macardoso said:


> Only limitation is that is uses a LOT of steam/compressed air, so you need to have a good compressor to run it. Mine may not be able to keep up continuously.



So this entire project is just to justify a new compressor?
Jeez....the lengths some guys won't go!




macardoso said:


> I've learned more about machining doing this engine than all of my projects before it combined. Seriously



I do NOT doubt that in the least.
....and I appreciate you bringing us all along. I have learned from it too!

-brino


----------



## macardoso

brino said:


> So this entire project is just to justify a new compressor?
> Jeez....the lengths some guys won't go!
> 
> 
> 
> 
> I do NOT doubt that in the least.
> ....and I appreciate you bringing us all along. I have learned from it too!
> 
> -brino



Lol. The real kicker would be justifying building a steam boiler to run this. I might leave that to my buddy. I will miss working on this, but I am also looking forward to checking this off my project list so I can start on some new ones!

I enjoy sharing this stuff and it really keeps me going.


----------



## macardoso

AHHHH S***.

Spun the jog pendant, had it set to the wrong axis.


----------



## Boswell

macardoso said:


> Spun the jog pendant, had it set to the wrong axis


Never happened to me.    (well, not recently ... as in this week )


----------



## Lo-Fi

Oh no, that's a bit gutting! What's the plan?


----------



## ErichKeane

Fortunately PM research is really good about selling replacement castings fairly affordably. Alternatively you could turn one from some brass rod if you were ok with losing the casting marks.


----------



## brino

macardoso said:


> AHHHH S***.
> 
> Spun the jog pendant, had it set to the wrong axis.



I was there Sunday! (.....unlike @Boswell, apparently)

I had moved the X-Y-Z feed select lever from Z-axis to X-axis to be able to move the table manually........it drags a little when trying to turn the same axis manually....... in order to drill a hole.

Luckily I did NOT have the drill bit low enough to contact the work.....so no harm but my ego......

It is "par for the course" as they say......the only people that never fail are the ones that don't do anything.

-brino


----------



## Manual Mac

Man, that sucks.
I think we’ve all done something like this.
At least you’re not bleeding.
Yeah, i’ve done that too......


----------



## Boswell

I usually end up snapping off an end mill or edge finder when I get the axis switch wrong. At least you only trashed the part. (trying for the bright side)


----------



## macardoso

Lo-Fi said:


> Oh no, that's a bit gutting! What's the plan?





ErichKeane said:


> Fortunately PM research is really good about selling replacement castings fairly affordably. Alternatively you could turn one from some brass rod if you were ok with losing the casting marks.



Called up PM Research and got a guy right at closing time. Very professional company. Guy was able to immediately confirm they had the spare castings in stock ($28). Got one, plus some of their old-timey 1/4-20 screws to match the blunder on the base, plus shipping for $40.

Still mad at myself but the ending was OK.

The amazing part is my Alu-Power endmill ($30) is perfectly fine after plunging into the part at probably 150 ipm. 

I gotta be careful about working in the shop after I finish my day job. I really need to be in the right headspace or I make mistakes. Really thought I was but I was shown differently.


----------



## Boswell

It is sooo hard to keep the right level of concentration on a repetitive task. I am sure all of us have ways to reduce risk but I thought that I would like to share a few things I do as we can never have too many safety discussions. Mardardoso, This is in no way a criticism but just an opportunity to discuss safety with our community. 

 I try to do repetitive tasks the same way in the same order as much as possible 
 I try to review common or possible failure modes in my mind at the beginning of a session. (easy to say, harder to remember to do)
 Slow Down. This is the hardest for me. I spent my career in process improvement and speed is money. I try to be aware of when I am going faster through the steps and purposely pause and think about.  (most often right after I crash something or make a mental error  )


----------



## BGHansen

macardoso said:


> AHHHH S***.
> 
> Spun the jog pendant, had it set to the wrong axis.


Can you braze filler in place and distress the surface to look like a casting?  I have a project where I'm going for a sand-cast look in a steel part.  A needle scaler does a really nice job mucking up the surface to look like a casting.

Bruce


----------



## macardoso

BGHansen said:


> Can you braze filler in place and distress the surface to look like a casting?  I have a project where I'm going for a sand-cast look in a steel part.  A needle scaler does a really nice job mucking up the surface to look like a casting.
> 
> Bruce


I'm not going to toss the part, although I do plan on doing all work on the new casting.

I do not have a welder, oxy torch, or anything to allow me to braze it up. I'll have to find a friend at some point. The casting is bronze, so I'm guessing you probably can find bronze TIG rod. 

Although I guess "brazing" bronze to bronze is really welding since you melt the base metal.


----------



## tq60

Now you have a "practice" part...

Sent from my SAMSUNG-SM-G930A using Tapatalk


----------



## macardoso

New casting is in! The original one was quite crooked along the parting line and required hours of filing to clean up. This one is nearly perfect right out of the box. Just need to not screw it up!


----------



## Braeden P

any more progress?


----------



## macardoso

Braeden P said:


> any more progress?


Yes, have some of the features on the connecting rod done and I am finishing up the eccentric ring. I'd like to finish that one first since it also requires a slitting saw but will be easier to access than the connecting rod. Only 4 major parts left to finish including these.

Wife and I are trying to buy a house so a lot of my free time is being taken up by that.

I'll post a real update soon.


----------



## macardoso

I like to only have 2 projects going at a time and I really want to scrape in my mill so I have a push to finish this up!


----------



## Janderso

BGHansen said:


> Can you braze filler in place and distress the surface to look like a casting?


You beat me to it Bruce.
Great job on the PM #6.


----------



## Janderso

macardso,
You are very gifted.
I am convinced building these models will make a better machinist out of you.
I made a mistake of ordering the #7. I found I don't like working with such small parts.
My equipment is massive,(this is a family forum) better suited for the #6.
These can eat time as you have so carefully recorded. Maybe when I'm caught up on my to do list I'll try again.
Please keep posting your progress. Very well done sir.


----------



## macardoso

Janderso said:


> Can you braze filler in place and distress the surface to look like a casting?





Janderso said:


> You beat me to it Bruce.
> Great job on the PM #6.



Would have been a great option, but I have no hot work tools other than a soldering iron for fine electronics. I'm well tooled for precision machining, but zero welding stuff, sheet metal equipment, presses, etc.



Janderso said:


> macardso,
> You are very gifted.
> I am convinced building these models will make a better machinist out of you.
> I made a mistake of ordering the #7. I found I don't like working with such small parts.
> My equipment is massive,(this is a family forum) better suited for the #6.
> These can eat time as you have so carefully recorded. Maybe when I'm caught up on my to do list I'll try again.
> Please keep posting your progress. Very well done sir.



Thanks very much. This is a lot of work and has definitely pushed me to learn a lot. The #5 and #6 are a good size and none of the parts are all that small. Only downside is they need a big compressor or boiler to run them.



Janderso said:


> My equipment is massive,(this is a family forum)


----------



## macardoso

So I started on the new connecting rod but only got as far as facing the two sides. The next step is to drill and tap the bolt holes, then split the cap with a slitting saw. Since this requires flipping my mill head 90 degrees to the side, I opted to work on some other parts first.

The eccentric ring is the next big part needing to be done. I started with some hand filing to clean up the exterior flash then milled the two faces to size. I had the part sitting firmly on the parallels in the vise but still ended up with 0.003" of non-parallelism in the opposing faces so I think I need to inspect my parallels and vise to see if something is up. Thankfully this shouldn't affect function and I can always scrape flat if needed.




I didn't get pictures, but in a second setup, I faced the top of the bridge, drilled the connecting hole and oil hole, and drilled, tapped, clearance drilled, and spot faced the holes for the bolts which will hold the two halves together after slitting.

Next I tried out my new Tormach Slitting saw arbor for the first time on scrap aluminum and steel. The blade is 1/16" thick, 3" diameter, 30 tooth and is dish ground.




I got a full 3/4" depth into mild steel using a 1/2" pass followed by a 1/4" pass. The blade has some radial runout but nearly zero axial. The tormach holder is very nice and I suspect the blade itself has runout.




The part was indicated flat using a 0.0005" DTI on the spot faces and then the indicator was zeroed on one spotface.




The blade height was adjusted to zero on the indicator such that the top face of the blade was level with the spotface. The DRO was then set at 1/2 of the blade thickness below zero.




The slitting saw had no issue with the cast iron.




Here is the clearance I was working with.




And split.




A quick file stroke removed the bung of material left by the saw on the top piece.




And the 2 halves lined up perfectly.




Next operation is to bore the precision hole for the eccentric.

I read so many horror stories about slitting saws, but found this to go extremely well.

More to come - Mike


----------



## Janderso

macardoso said:


> So I started on the new connecting rod but only got as far as facing the two sides. The next step is to drill and tap the bolt holes, then split the cap with a slitting saw. Since this requires flipping my mill head 90 degrees to the side, I opted to work on some other parts first.
> 
> The eccentric ring is the next big part needing to be done. I started with some hand filing to clean up the exterior flash then milled the two faces to size. I had the part sitting firmly on the parallels in the vise but still ended up with 0.003" of non-parallelism in the opposing faces so I think I need to inspect my parallels and vise to see if something is up. Thankfully this shouldn't affect function and I can always scrape flat if needed.
> 
> View attachment 359515
> 
> 
> I didn't get pictures, but in a second setup, I faced the top of the bridge, drilled the connecting hole and oil hole, and drilled, tapped, clearance drilled, and spot faced the holes for the bolts which will hold the two halves together after slitting.
> 
> Next I tried out my new Tormach Slitting saw arbor for the first time on scrap aluminum and steel. The blade is 1/16" thick, 3" diameter, 30 tooth and is dish ground.
> 
> View attachment 359517
> 
> 
> I got a full 3/4" depth into mild steel using a 1/2" pass followed by a 1/4" pass. The blade has some radial runout but nearly zero axial. The tormach holder is very nice and I suspect the blade itself has runout.
> 
> View attachment 359518
> 
> 
> The part was indicated flat using a 0.0005" DTI on the spot faces and then the indicator was zeroed on one spotface.
> 
> View attachment 359519
> 
> 
> The blade height was adjusted to zero on the indicator such that the top face of the blade was level with the spotface. The DRO was then set at 1/2 of the blade thickness below zero.
> 
> View attachment 359520
> 
> 
> The slitting saw had no issue with the cast iron.
> 
> View attachment 359521
> 
> 
> Here is the clearance I was working with.
> 
> View attachment 359522
> 
> 
> And split.
> 
> View attachment 359523
> 
> 
> A quick file stroke removed the bung of material left by the saw on the top piece.
> 
> View attachment 359524
> 
> 
> And the 2 halves lined up perfectly.
> 
> View attachment 359525
> 
> 
> Next operation is to bore the precision hole for the eccentric.
> 
> I read so many horror stories about slitting saws, but found this to go extremely well.
> 
> More to come - Mike


You made this task look easy.


----------



## macardoso

Here is the rest of the Eccentric Ring:

The part was stood up on parallels and very gently clamped in the vise.



I wrote a simple boring routine. This way I could just adjust the boring head and hit cycle start over and over. 



Unsurprisingly the setup is not very rigid and I really had issues with my boring bars wanting to chatter. Ended up going with a brazed carbide bar that I ground to an aggressive rake.



Here is the bore finished. Tolerance is pretty generous so it was not hard to hit it.



And here it is with the eccentric. 

Looks great, but something was not right... The fit was very tight even though I left 1.5 thou clearance. 

Turns out my boring setup was very poor and even though the vise was clamped lightly, the part was deformed. The bore was cut a perfect circle, but when removed from the vise the sides sprung out into an egg shape. 

I figured my only chance at fixing it was to try to bend it back straight. This was done over several hours of very gingerly clamping each half of part in the milling vise and squishing it. Move a few degrees on the handle and remove and test the fit.



I was standing at the finish line and POP!

My heart sunk. The cap cracked at the midline right as I was dialing in the last few tenths. Maybe if I had gone slower I wouldn't have broken it, or maybe the part was incapable of bending as much as required. Either way it didn't matter. I don't remember ever wishing life had an UNDO button quite so much.




Anyways, I got 2 new castings from PMR at $4 each. Started facing them and realized I was having accuracy issues due to my vise. Took a 40 hour hiatus from the steam engine to correct the inaccuracies in the vise so hopefully I can make better parts.









						Scraping my Shars 4" Milling Vise
					

Been working on a steam engine and really been having a hard time holding parallelism on parts where one side is machined and then flipped onto parallels in my milling vise. I finally stuck an indicator in the spindle and tested the vise and found it to be almost 4 thou out of flat with the...




					www.hobby-machinist.com
				




I still need to repeat the drilled holes, slitting, and boring, but this time I will be using a different setup, hopefully with better results.

Stay tuned - Mike


----------



## Peyton Price 17

my neighbor used to bore out airplane engines on a jig bore. one cylinder a day and a 150k an engine. he also used to run a CNC to machine caps for oil rigs and the part was the size of a car and cost the same as a house. I'm pretty sure both places were bought up and taken down.


----------



## macardoso

Peyton Price 17 said:


> my neighbor used to bore out airplane engines on a jig bore. one cylinder a day and a 150k an engine. he also used to run a CNC to machine caps for oil rigs and the part was the size of a car and cost the same as a house. I'm pretty sure both places were bought up and taken down.


Well if my successes in this project tell you anything, I'd be out of business. Thankfully this is all for fun and learning.


----------



## ErichKeane

Ouch.... is it bad I predicted that ending?  I would suggest putting it on a pallet of some sort.


----------



## macardoso

ErichKeane said:


> Ouch.... is it bad I predicted that ending?  I would suggest putting it on a pallet of some sort.


Yeah, already headed down that path for the second one. Sometimes you have to learn lessons the hard way.

As a bonus, strapped down to a pallet will make the whole setup more rigid and less likely to chatter during boring.


----------



## Janderso

macardoso said:


> I still need to repeat the drilled holes, slitting, and boring, but this time I will be using a different setup, hopefully with better results.


Looks great!!
Well done.


----------



## tq60

You may also have stresses complicating things.

Well before finish stop, measure then release pressure and see if it moves.

May need to bang on it to stress relieve it.

Getting it back into vise a challenge but a coax indicator could help.

Sent from my SAMSUNG-SM-G930A using Tapatalk


----------



## macardoso

Opted to do a bit of CAD/CAM for the Eccentric Fixture. Not that is absolutely necessary, but it has been a good while since I've opened the program and I wanted the practice.

First I modeled the critical features for boring.




Next I modeled the piece of aluminum scrap I'm working with, including the randomly placed hole in it.




Additional features were added to help place the hold down fasteners




Locations for clamping washers are sketched in.



Clamping Bolt locations are drilled and Tapped. The central bore is expanded.



Gcode is written



Finally, the fixture was machined. and hand tapped











Next step is to load the part onto the pallet and bore the hole.


----------



## Janderso

macardoso said:


> Opted to do a bit of CAD/CAM for the Eccentric Fixture. Not that is absolutely necessary, but it has been a good while since I've opened the program and I wanted the practice.
> 
> First I modeled the critical features for boring.
> 
> View attachment 363032
> 
> 
> Next I modeled the piece of aluminum scrap I'm working with, including the randomly placed hole in it.
> 
> View attachment 363033
> 
> 
> Additional features were added to help place the hold down fasteners
> 
> View attachment 363034
> 
> 
> Locations for clamping washers are sketched in.
> View attachment 363035
> 
> 
> Clamping Bolt locations are drilled and Tapped. The central bore is expanded.
> View attachment 363036
> 
> 
> Gcode is written
> View attachment 363044
> 
> 
> Finally, the fixture was machined. and hand tapped
> 
> 
> View attachment 363065
> 
> 
> View attachment 363066
> 
> 
> View attachment 363068
> 
> 
> Next step is to load the part onto the pallet and bore the hole.


Using a CNC mill is cheating. I'm just wishing I was smart enough to use Fusion 360 and applying the draft to the mill.
Nice work, even if you cheated


----------



## macardoso

Janderso said:


> Using a CNC mill is cheating. I'm just wishing I was smart enough to use Fusion 360 and applying the draft to the mill.
> Nice work, even if you cheated


100% not necessary for the engine. The CAD/CAM/CNC workflow is complicated and it was a good opportunity to stretch those muscles. 

Automating the boring process is SOOOOO nice lol. I can start it and read a book for a minute at a time as it is cutting.


----------



## macardoso

Janderso said:


> Using a CNC mill is cheating. I'm just wishing I was smart enough to use Fusion 360 and applying the draft to the mill.
> Nice work, even if you cheated


Also, the whole CNC thing isn't too hard to jump into. You can get cutting pretty quick, but it takes a while to start to feel like you know what you are doing. I've got 8 years in, know how to make complicated parts (moderately quickly), but I still hand code lots of stuff that more experienced guys would bang out with canned cycles, subroutines, offsets, scaling, etc.


----------



## Janderso

macardoso said:


> more experienced guys would bang out with canned cycles, subroutines, offsets, scaling, etc.


English please, this is a family forum.


----------



## hman

I still hand code most of what I do on my EDBD CNC mill.  Tried using the CAM portion of Fusion 360, also tried CamBam.  Yes, they work ... but the tool paths and sequences of operation they choose to do look frustratingly inefficient.  WAY too much time wasted cutting air!  So far I haven't had to use very much of the "canned cycles, subroutines, offsets, scaling, etc.," though I'm trying to learn.  And if nothing else, it's a lot of fun to stretch the muscles (between my ears)!


----------



## Boswell

hman said:


> WAY too much time wasted cutting air!


When I first got my CNC Mill working, I used CamBam and was also frustrated by the inefficient tool paths. For one-off parts, I did not think it mattered much, but when it did matter, like for higher quantitates, I used CamBam to generate the basic code and then I modified it by hand to reduce the cycle time. This seemed hybrid technique worked well for me. However, I no longer use CamBam and have moved on to BobCad and have not felt the need to hand modify any code.


----------



## macardoso

I hand code very simple operations (drilling, facing, etc.) but have used CAM for most else. Over the years I've tried:

-MeshCAM
-HSM Works
-Mastercam 9
-Mastercam x8
-Mastercam 2017

Meshcam was super basic but dirt simple to use. Got me going in the early days, although it is not efficient and cannot make trochoidal "high efficiency" toolpaths.

HSM Works was included in Inventor for a while so I used that. 

I have been fortunate enough to have access to MasterCAM for some time so that is what I use for the most part. If I were just getting into it, I don't know if this would be my first choice (ignoring price) as it is somewhat complicated, but it is a very powerful and flexible program. I never get air cutting unless I intentionally add it.


----------



## macardoso

Finished the Eccentric Ring - very happy to have this one done!

Fixture worked pretty well, much better than before but I should have made some custom clamps to go with it rather than bolts with unsupported washers.

First, only the bottom side of the split ring was clamped.



Then the flat faces were indicated and tapped into alignment with the Y axis within 0.0005". This is critical to make sure the bore is split down the middle and not a chord. I also used an electronic edge finder at this point to locate the spindle on the split line. 
	

		
			
		

		
	




Next boring was done. Between a thicker boring bar and better clamping the process went much better, but chatter was still a real problem. I ended up hand sharpening the boring bar on a diamond lap to get a very sharp positive cutting edge. I also was adjusting the spindle speed while the machine was running both up and down whenever it started to chatter. By varying the feed/speed constantly I was able to avoid too much chatter. 



Here is the complete bore right before removing it from the fixture



And here is the finished Eccentric and Eccentric Ring. They must be carefully assembled to get the split lines to align otherwise the bearing is not smooth, but if they are well aligned the motion is buttery smooth.


----------



## Janderso

Oh man, that's cool!


----------



## Philzy

Thanks for posting this. I’ve had this same model sitting in a box for months. Decided it was too much for my little 7x16 lathe to handle. Waiting on my new Precision Mathews before I get started.


----------



## Janderso

Philzy said:


> Thanks for posting this. I’ve had this same model sitting in a box for months. Decided it was too much for my little 7x16 lathe to handle. Waiting on my new Precision Mathews before I get started.


How's the smoke up there in the Pacific North West?
I heard you were getting smoke from the California fires??


----------



## macardoso

Philzy said:


> Thanks for posting this. I’ve had this same model sitting in a box for months. Decided it was too much for my little 7x16 lathe to handle. Waiting on my new Precision Mathews before I get started.


Hope you enjoy it! Wife and I are in the process of buying our first house and mine has been sitting in the box with only the connecting rod remaining. Need to finish this puppy!


----------



## Janderso

macardoso said:


> Hope you enjoy it! Wife and I are in the process of buying our first house and mine has been sitting in the box with only the connecting rod remaining. Need to finish this puppy!


Good luck on the house. may you have many years of health and happiness.


----------



## Philzy

Janderso said:


> How's the smoke up there in the Pacific North West?
> I heard you were getting smoke from the California fires??


I don’t have to worry about the smoke from California. I’m getting more than enough WA smoke.  Five fires within a 60 minute drive of my house.


----------



## Janderso

Philzy said:


> I don’t have to worry about the smoke from California. I’m getting more than enough WA smoke.  Five fires within a 60 minute drive of my house.


Ooohg 
So sorry to hear that. I hope you are OK.


----------



## macardoso

Whew! Made a big push on this yesterday and got the connecting rod done. We are in the process of packing the house for our move and this was the last thing I wanted to get done before the machines come out of the basement and got wrapped up to go on the truck. Took a vacation day off work to get a full uninterrupted day.

I had previously spent 2.5 hours on the first connecting rod before fumbling the keyboard on my CNC and crashing an endmill into the part. Then another 3 hours on this one, hand filing the general shape and facing the two sides of the split end of the rod to thickness and parallelism. 

I found this part particularly tricky to fixture. There are no flat sides on it, the main shaft section is somewhat twisted and tapered, and when you do clamp it, the part sits crooked in the vise. Furthermore at ~8" long, this takes up a lot of space on my mill and requires work on both ends accurately clocked to eachother.

I opted for a poor man's compound angle vise. I placed a 3.5" drill press vise in my 4" milling vise, and a 2" tool makers vise in that one. This did 2 things. First it allowed me to dial in the part's orientation one axis at a time without affecting the orientation of other axes during adjustment. Second, it gave a fair bit of clearance above the table for the next operation. I'll explain why this was necessary when we get there.




It took me most of the morning to get the part clamped securely and indicated true. The part is held in the tool makers vise using a pin and some shim stock to improve the clamping rigidity. A trick that I use a lot is to use a round object (in this case some 1/2" steel stock) on the moving jaw of the vise to grip on parts which have uneven or non-parallel faces. Without this, the moving jaw couldn't securely grip on the part. I then indicated the pitch of the part (about the X axis) first by tapping the tool makers vise in the jaw of the drill press vise. Then I securely tightened the drill press vise and started tapping it in the jaws of the milling vise to set the roll of the part (about the Y axis). The milling vise was then tightened securely. Finally the milling vise was rotated on the table surface to set the yaw of the part (about the Z axis). All indicator readings were made within 0.0005", probably excessive for a casting, but I didn't want any screw ups.




My mill has 9" of table to spindle clearance, which left no possibility of doing the end work on the cap with the part vertical. This required flipping the spindle 90 degrees on its side to access the side of the part. I took a lot of time to carefully position the fixture on the table to allow room for the end work on the one side, as well as all later operations from the vertical position in one setup. This unfortunately left extremely little room to work requiring a rather complicated setup to square the mill head to the face. I used the side of my precision granite square (less accurate, but still guaranteed square on the instrument certificate) to indicate off of. Once the spindle was square within 0.0002" TIR of a 2" swept circle, I could edge find the cap screw locations.







The screw holes were spotfaced, center drilled, clearance drilled (to half depth), and tap drilled through. Following that, a 3" 1/16" thick slitting saw was used to split the cap. I didn't get a picture of the slitting operation, but the tool makes an appearance later. At this low speed (150 rpm) and uneven loading (slightly eccentric slitting saw) the servo spindle struggles with the cut. It only consumes about 10% of the motor torque, but it would stall and surge significantly. Higher speeds and feeds actually do a lot to fix this problem.




After slitting the tap drill holes were tapped. I wish I had done this before slitting since the tap raised a burr, but it wasn't the end of the world




Using a tenths indicator and an optical flat, I precision edge found the split line for subsequent drilling. Joe Pie has a great YouTube video on this method. The cap was screwed back on and I used some sharp drills to open the hole up.




Thinking it might cut a bit more freely on this poorly supported part, I tried to expand the hold with a 3/8" 3F aluminum specific carbide endmill. Unfortunately it snagged immediately and destroyed the endmill. There's $40 down the drain. Fortunately the part was fine and I drilled the hole out to 3/8"




I then wrote a short multi-line MDI program on the CNC to repeatedly bore the hole and retract. I advanced the diameter 10 thou at a time. Final dimension was 0.5001" (.5000 target, reamed, no stated tolerance). The crank pin was turned to 0.4988"




I test fit the crank shaft in-situ and the fit was perfect. Would not be able to easily line this up again to correct the bore once it was removed from the machine.




The other end was drilled and reamed to 0.3135" for a sliding fit to a 0.3125" pin. The prints called out facing both sides of this joint, plus a square bottomed slot with precision width and depth. The alignment to the other end is absolutely critical or the assembly will bind. For these reasons, I opted to not move the part from the fixture at all and complete all the remaining operations with the slitting saw. This guarantees alignment, although the cutting process was VERY slow.

I took about 45 minutes to quadruple check all my Z position math for the slitting saw since I'd be creating finished dimensions in one shot using both the top and bottom of the saw blade.




At this point, I had faced both the top and bottom sides (dimension within 0.0010" of nominal) and the slot width (within 0.001" of nominal). Unfortunately the 3" saw was too small to give the full slot depth required. 




I revisited the cut with a 4" diameter 1/16" thick slitting saw. Taking many passes in the Z direction, each less than the blade width, I was able to mill the slot to full depth, with a flat bottom. The finish was actually perfect, and you can't tell I worked at it through many passes.







Here I checked the fit to the cross head. The fit is very nice, albeit just a smidge tight. The crosshead bearing faces that rub on the inside of the connecting rod were machined slightly out of parallel previously. The fit is still very buttery smooth and will likely loosen up just a bit as things wear in.




All in all, this took 8 hours yesterday, and a total of 13.5 hours including the scrap part.


----------



## ErichKeane

That optical flat method is interesting... though I guess I would have just found the split-line by removing the cap, using an edge finder, then re-adding the cap back.


----------



## macardoso

ErichKeane said:


> That optical flat method is interesting... though I guess I would have just found the split-line by removing the cap, using an edge finder, then re-adding the cap back.


Yup, probably a sane person would do that. I don't trust my edgefinders much better than 0.001". If you don't drill and bore right on the split line, you end up splitting the cap on a chord of the circle. With such little clearance between the parts, it doesn't take much for you to not be able to assemble the parts. The indicator method is as accurate as your indicator (0.0001"). The optical flat can be replaced with any good and flat surface (carbide insert, gage block, etc.) but I have a small flat for stuff like this ($20 on ebay).


----------



## macardoso

Here is the engine as it stands today.




The connecting rod now links the crankshaft with the piston side and allows you to manually cycle the engine. Even though a good alignment fit hasn't been done yet, everything slides really smoothly and there is not any appreciable rubbing or binding.

There are no seals installed in the packing nuts and the piston has no rings installed. Only some computer paper head gaskets were made. Even still, the whole thing is nearly gas tight. You can hear the air being pumped in and out of the cylinder through the steam inlet port, and blocking this port with your finger makes it so you cannot turn over the crankshaft.

I have technically made all the remaining parts, but they require a fair bit of hand fitting. The next steps will be to bend the valve rod, pin it to the linkage joint, and set the valve throw and timing. With that complete, the engine should be ready to run on shop air.

My buddy (who I have been making this for) took it home to mess around with and show his father. I'm going to get it back from him before I move so I can put the finishing touches on it. Specifically, the frame needs a hole drilled for an oil cup, the cylinders need drain bung holes drilled and tapped (necessary if the engine would ever be run on live steam), and we came up with a plan to add oiling provisions to the eccentric and connecting rod (crankshaft side). I'll then tune it up and run it in for several hours to make sure it works well. I'll also install all the seals and proper gaskets. I also want to adjust the fit of the crankshaft bearings, and the inboard head of the cylinder as these are the locations of the most rubbing. My friend plans to clean it up, polish it, and paint it with a classic green enamel.

Here is a list of machined parts and my status:

Crank Disc (Qty. 2): *Done (4.5 hours)*
Cross Head: *Done (8.5 hours)*
Crank Pin: *Done (4 hours, 1 Scrap)*
Lower Valve Head: *Done (2 hours)*
Piston Rod Packing Nut: *Done (1.5 Hours)*
Lower Linkage: *Done (2.25 Hours)*
Upper Linkage: *Done (2.25 Hours)*
Eccentric Hub: *Done (8 Hours, 1 Scrap)*
Wrist Pin Bolt and Nut: *Done (1 Hour)*
Outboard Valve Head: *Done (2.75 Hours, 1 Scrap)*
Valve Rod Packing Nut: *Done (1 Hour, 1 Scrap)*
Oil Cup (Qty. 2): *Done (1.75 Hours, 1 Scrap)*
Piston: *Done (5 Hours)*
Lower Valve Rod: Done pending final fit (0.5 Hours)
Pillow Block & Cap (Qty. 2): *Done (17.5 Hours)*
Valve Eccentric Ring and Cap: *Done (10 Hours, 1 Scrap)*
Upper Valve Rod: Done pending final fit (0.5 Hours)
Valve: *Done (3 Hours)*
Crankshaft - Short: *Done (0.75 Hours)*
Crankshaft - Long: *Done (0.75 Hours)*
Piston Rod: *Done (4.5 Hours, 1 Scrap)*
Connecting Rod and Rod Cap: *Done (13.5 Hours, 1 Scrap)*
Base: *Done (5.5 Hours)*
Flywheel: Buddy did this one, I just skimmed it true. *Done (1 Hour)*
Frame: Done pending drip oiler selection (10 Hours including repair)
Cylinder: In Process, drain port needed (9.5 Hours)
Inboard Head: *Done (3.5 Hours)*
Head: *Done (1.5 Hours)


Recorded hours to date: 126.5 Hours *(probably close to 140 including cleaning, bench work, and planning)
*Estimated Completion: 95%*


----------



## Manual Mac

Thanks SO much for taking us on The Grand Tour of this build.
I’ve thoroughly enjoyed it so far and appreciate your documenting it for us.
Good luck with your move.


----------



## macardoso

Manual Mac said:


> Thanks SO much for taking us on The Grand Tour of this build.
> I’ve thoroughly enjoyed it so far and appreciate your documenting it for us.
> Good luck with your move.


I love this community and sharing here has helped me get the kicks in the tush that I need from time to time to keep moving on longer projects. I've also learned a ton here and hope I can contribute a little bit back.


----------



## wachuko

As a newbie, the scary part of these kits is the amount of jigs that have to be made to just work a part... This is very intimidating for me...

I am so grateful for you taking the time to share the process... all of it, the good, the bad, and the ugly... 

Good luck with the move!!


----------



## macardoso

wachuko said:


> As a newbie, the scary part of these kits is the amount of jigs that have to be made to just work a part... This is very intimidating for me...
> 
> I am so grateful for you taking the time to share the process... all of it, the good, the bad, and the ugly...
> 
> Good luck with the move!!


I think the workholding is absolutely the most difficult thing about working with castings. Mill vises are great for bar stock but suck at holding oddly shaped parts. I'll say that ~75% of the time I have spent on this engine has been setup and fixturing.  Lots of time with an indicator making sure things are lined up. Really gets you thinking about the best way to do things, any ways you can do more operations in one setup, etc.

I'll say that this project has single handedly pushed my machining skills and knowledge further than anything that came before. Kinda cool.

My only aversion to picking up another one would be the time commitment. Being 27, between work and family, I don't get much shop time at all in a week. So a 150+ hour project just drags on forever. I also am uncomfortable with outstanding projects, so I am always wanting more time to get it done.


----------



## Lo-Fi

wachuko said:


> As a newbie, the scary part of these kits is the amount of jigs that have to be made to just work a part... This is very intimidating for me...



You'll get to appreciate that making jigs, fixturing and workholding is actually the fun part 

I've been making a tool and cutter grinder from castings myself. Had a few "lessons" (mishaps) as it's my first time working with rough castings. 
My top tips would be: 
Watch Joe Pie on YouTube. His lathe project in particular, though his approaches in general tend toward using fixtures and jigs to make life easier for yourself regardless.
If the grip is smaller than the chip, the part will slip. 
Order of operations is key. Set yourself up so you've got access to do all the things you need to do in a specific orientation in one setup if you can. 
Think carefully about how you can used the features you're machining to register features that come later.

Don't be afraid of stuff you can't just sling in the vise! It's really rewarding to set up a jig and absolutely nail some parts. Certainly more than doing something quick but sketchy and getting a mediocre result or failing altogether. Joe Pie is an absolute master of this and the best content I've seen for consistently inventive, effective setups that get excellent results. Taught me a lot about how to think about setups.

Loving your work, @macardoso


----------

