Tube Polisher....

[JimDawson]

Moving right along.... OK, I just got back to this project.

Just a reminder of what this part looks like, a cutaway view


I couldn't find an endmill in the shop that had a flute length long enough to rough out the pockets on the mill, so I just decided to bore the internal features on the lathe. Only took a few minutes, probably faster than roughing then boring in the mill. Got to use my new insert boring bar set. I'm happy with the set, worked well.



And finish bored


So next is drill & tap the mounting holes. Find 0 with the Blake. I've had the Blake indicator since the 80's, I use it all the time, makes finding hole centers a breeze.



On the drawing I show the holes through, but actually drilled 1'' deep. I had to order some drill bits, I couldn't find any #5 drills in the shop. My prefered drill bit size for 1/4-20 taps. Spiral flute machine tap, but hand tapped by putting the spindle in neutral, I normally do it this way on blind holes.


Now I need to clock the next operation to the mount holes, so need a way of locating the part. I did it differently than the original plan, much simpler. First mill a flat surface in the soft jaws


and then put a screw in two opposing holes.


Then just lay the part down and tighten the vice


I couldn't reach all the way down to the center with my edge finder, so any convenient spacer works fine. I had a 123 block sitting within arms reach, so that made the perfect spacer to measure from.


Then chew out the parts I don't want. 3 flute, solid carbide aluminum rougher, 2100 RPM, 206 SFPM, 8.5 IPM, 0.0014 feed/tooth. Full DOC, 0.05 stepover, adaptive toolpath, mist coolant. About 16 minutes/part



And done


I have a couple of spacers and bearing retainer plates to make, simple little parts, and bore the flywheel to 75mm. Then that will complete the parts for the main drive assembly. I'll get to those in the next day or so.

 

[mattthemuppet2]

that's a neat trick for finding the edge of a cylinder, thanks!

 

[Papa Charlie]

Looking great. Nice trick. Thanks for sharing.

 

[Papa Charlie]

How is the project coming? Hope all is ok, been awhile since your last post.

 

[JimDawson]

How is the project coming? Hope all is ok, been awhile since your last post.

It's coming along. Been working on some other stuff, but I have a bit more done, but nothing really post worthy. I have all of the parts on a pallet right now and am starting the assembly process.

 

[JimDawson]

I got some work done, got the flywheel bored to 75mm to accept the center shaft. And got the pinion shafts completed.
Not much to see here....But



Then on to the main bearing spacer. Not a complex part, but rather a pain to make. 2.95ID x 3.75OD x 0.030 thick. I forgot to have this laser cut in the last batch of laser parts, so I'll make it on the mill.



It goes between the two main bearings to allow cinching up on the inner races and keeping the outer races apart. That way I'm not axial loading the bearings.



So how do you hang onto a piece of 0.030'' steel and machine it? Well, there are several ways, but this is the way I did it for this project.

Where possible I like to sandwich the part between two sacrificial pieces, in this case I used 3/4 MDF, because that's what I had within arms reach. Could have been aluminum or even steel. If holes in the finished part were not allowed, then I would have used a different holding method, possibly doing the ID on the mill and the OD on the lathe using the mating part as an arbor.

I have a bunch of 6.25 x 5.188 x 0.030 steel pieces on the shelf, so first cut a couple pieces of MDF about that size. Then make a quick drawing and CAM layout to generate the toolpaths. Spiral down cut, 0.5 degree angle. 5/16 endmill



Sandwich the metal between the MDF pieces and clamp


Drill for screws and secure with 1 5/8 deck screws.


A light cut to test the end mill/screw head clearance, no problem



Everything looked good until it got to the steel on the first pocket. The feed and speed were too high and it threw some sparks, an almost new solid carbide, 4 flute end mill. Hmmm, not good. And the cutter sounded odd as it finished that cut. So I paused the machine when it moved to the inside cut and found steel built up on the cutter, basically jaming up the flutes. Never seen steel do that before, but this is some really gummy steel. Anyway the cutter looked OK after I cleaned out the steel, only a couple of small chips, good enough for this project. So I let it finish the cut after reducing the speed to 115 SFM and 5 IPM on the feed. The inside pass cut fine with the expected slight burr from the damaged endmill.

I'm not using coolant here, just using the air blast.


This is what I found when I remove the outside clamp. The cutter build up had rolled the edge of the material over and things got a bit warm also. Yeah, that's a pretty dramatic burr.



Since the OD dimension is not critical, a little work on the disk sander made quick work of the burr. I couldn't run a smaller tool path because the screw heads would have been hit by the endmill, I only had a few thou clearance.

And the finished product.



Everything would have been fine but I thought that the 175 SFM and 11 IPM was a reasonable feed and speed for the job, pretty conservative actually. I cut some slots in some A36 steel tubing yesterday using that same endmill using that feed and speed, 1/4'' deep in one pass. No problem, but I was using a trochoidal tool path rather than a spiral down toolpath. The tool path makes a lot of difference in the way material cuts, I was also using coolant.

Anyway the job got done and the result was satisfactory, and that's what is important.

 

[7milesup]

Nice work Jim. I am always interested in how experienced guys fixture their material. I recently did a part where I utilized some sacrificial plywood underneath it but was unsure if that was a "proper" way of doing it, so thanks for showing the fixturing.

 

[JimDawson]

Nice work Jim. I am always interested in how experienced guys fixture their material. I recently did a part where I utilized some sacrificial plywood underneath it but was unsure if that was a "proper" way of doing it, so thanks for showing the fixturing.

Thank you.

IMHO, in machining, as long as shop safety is observed there is no ''proper'' way of doing anything, but rather there is what works for the job at hand. In most cases wood products work pretty well for temporary fixturing, and sometimes are even appropriate for production use. My go to material is MDF, easy to work with, dimensionally stable, oil resistant, and inexpensive.

It's my pleasure to pass on my experiences.

 

[Papa Charlie]

Great job Jim, material sounds like it is pretty soft. Have had trouble with soft metals on my lathe. Had to slow things down, feed and depth of cut to get a reasonable finish. Prefer harder metals if given the opportunity.

Thanks for sharing.

 

[Boswell]

I have used spoil boards before, but never thought to sandwich a thin part between two spoil boards. Thanks for the tip Jim.