# A Question On Machining



## prasad (Oct 20, 2016)

Guys

I started working on a small project of making a small turn table arrangement using an aluminum material. The OD of the disc is close to 6 inches and thickness at the edge is about 0.2 inch. To help me mount it on a stepper motor shaft I thought of having a thicker boss at the center of thickness 0.5 inch. I mounted the rough cut aluminum disc on my 4-jaw chuck and machined one face and got the round boss and finished surface as you can see in the photo below. 
	

		
			
		

		
	




I then removed it from the chuck and mounted it back on the 4-jaw gripping the boss that I had just made, trued it. and then did the facing operation until I got a decent smooth surface finish. The last operation, I drilled a hole in the center to suit the motor shaft, a small interference fit.



Here is my problem. When I turn the motor I find the turntable is not running flat. Its top surface wobbles. Apparently the hole did not go straight. How can that be? Where did I go wrong and what should I do to eliminate the wobble?

Thank you
Prasad
Eastern PA


----------



## jim18655 (Oct 20, 2016)

Did you true the front surface or only the center? You would need to make sure the front surface is running flat - 90 degrees-  in relation to the drill.


----------



## Bill Gruby (Oct 20, 2016)

When you chucked that part in the chuck did you indicate both the OD and the face ?If you did not indicate the face as being flat, (true),  the hole is probably at an angle which will cause the wobble.

 "Billy G"


----------



## Wreck™Wreck (Oct 20, 2016)

You turned it around in the chuck? Your goal is to keep the flat face and the bore concentric correct, face the flat side then bore in the same set up. Flip and turn the back side and the boss as a second operation. Always try to do related features in the same set up.


----------



## Bill Gruby (Oct 20, 2016)

The post by Jim was being done as I was doing mine. At least they are both in agreement.

 "Billy G"


----------



## mikey (Oct 20, 2016)

Assuming you indicated the part so it is running true, then the center of the part should be on the spindle centerline. If the tailstock or drill chuck is not aligned with the spindle centerline then it will drill off and you get wobble. To compound matters, the drill will not drill a truly round or straight hole. If you need a round hole then it needs to be bored or reamed. Since you need it round and straight the best choice would have been to bore the hole. 

My suggestion is to make another part, indicate it accurately in the chuck, bore the center hole and face the part. Any inaccuracy from the drill, drill chuck or tailstock is thus eliminated.


----------



## prasad (Oct 20, 2016)

I indicated it on both - machined side face (which was facing the chuck)  and diameter. The non-machined side (face of the disc) was now ready for facing cut. That was how I got truly flat disc. I measured the thickness using my Mitutoyo micrometer and the two faces were truly parallel to less than 0.25 thousandths. 

Yesterday I started doubting if the the job held in the chuck may have moved in the chuck when I started the drilling operation. So I once again held it in the same chuck, took extreme care to true it on face and diameter. The indicator showed less than 0.25 division. In this condition I ran the lathe and ran the drilling operation (pushed the same drill bit in). It went in and did not cut any material. That indicated that the job did not get displaced during the drilling operation. However the hole does not appear square to the surface. 

I am truly confused.


----------



## Tozguy (Oct 20, 2016)

Drilling is not for making a concentric bore as already mentioned.
Hole should be bored or reamed. Can you bore over size and bush the hole back to size?


----------



## prasad (Oct 20, 2016)

mikey said:


> Assuming you indicated the part so it is running true, then the center of the part should be on the spindle centerline. If the tailstock or drill chuck is not aligned with the spindle centerline then it will drill off and you get wobble. To compound matters, the drill will not drill a truly round or straight hole. If you need a round hole then it needs to be bored or reamed. Since you need it round and straight the best choice would have been to bore the hole.
> 
> My suggestion is to make another part, indicate it accurately in the chuck, bore the center hole and face the part. Any inaccuracy from the drill, drill chuck or tailstock is thus eliminated.



Thanks Mikey, that makes some sense. It is possible that my TS or drill chuck held in the TS is not aligned with the spindle. I am not sure if I can bore a 5mm diameter hole. However I do find McMaster selling 5 mm reamer. I will order one. I will also do the reaming by hand first, then mount it in the chuck, indicate it as best as I can before facing. I have to get new stock too.


----------



## Bill Gruby (Oct 20, 2016)

Is that a typo, 0,25?? 0.25 is 1/4 inch, or am I not seeing something??

 "Billy G"


----------



## mikey (Oct 20, 2016)

May I suggest that you go on ebay and find a small boring bar? Micro 100 sells some really nice ones that will do this job easily. 

The reason I suggest boring is because a reamer will follow a crooked hole. It will have a nice finish but the hole may not be straight. A boring bar will cut the hole straight AND give you a good finish; how accurate the bore will be depends on your skills when you bore it.


----------



## Wreck™Wreck (Oct 20, 2016)

Are you using inch or metric measuring tools? There is a considerable difference between .o25 MM and .025 inches, 25.4:1 exactly.
.025MM is 0.0009 inches.

Or as my delightful Windows Calculator tells me. 9.84251968 to the -4


----------



## mikey (Oct 20, 2016)

prasad said:


> Thanks Mikey, that makes some sense. It is possible that my TS or drill chuck held in the TS is not aligned with the spindle. I am not sure if I can bore a 5mm diameter hole. However I do find McMaster selling 5 mm reamer. I will order one. I will also do the reaming by hand first, then mount it in the chuck, indicate it as best as I can before facing. I have to get new stock too.



Before you go making a new part, would it be possible to bore out the center and press fit a bushing it it? If so, you can drill and bore the bushing, reface the part and you're done.


----------



## prasad (Oct 20, 2016)

Bill Gruby said:


> Is that a typo, 0,25?? 0.25 is 1/4 inch, or am I not seeing something??
> 
> "Billy G"



I do everything in inches but the stepper motor I have has a 5 mm shaft. I measured it to be slightly larger than 5 mm. I ordered a 5 mm drill bit that I used for drilling.


----------



## Subwayrocket (Oct 20, 2016)

Hope you get it straightened out !  Is this a welding turntable ?  
As a last resort, you could also weld that hole closed and start over ...although the welding might cause distortion across the large flat disc . Need alotta chill blocks ...
Nice project either way !
I'd love to see the plans .
All Too often I could use a turntable for welding.

Steve , Northeast PA ...coal country


----------



## RJSakowski (Oct 20, 2016)

If your tailstock is slightly off center, the drill bit may find the center but can cut at an angle.  The angle won't be much but being magnified by the  6" diameter will create a fair amount of wobble.  The tailstock, including the drill chuck must be aligned with the spindle, both horizontally and vertically.  Additionally, the drill bit must be straight.  Both drill bits and reams are fairly flexible.  A ream tends to follow a drilled hole so it will not correct a hole that is misaligned.

For precision alignment, I would bore the hole.  You can make a micro boring tool from a broken tap or drill bit. Had one for years that I used to bore holes as small as .1" diameter.  Drill a pilot hole as large as you comfortably can without cutting into the finish diameter.  You will be able to make a precision diameter hole which is true to your disk.  If you don't have a set of pin gages, turn some test pins which are slightly smaller in diameter that your finish size to allow you to sneak up on the final size.  Use a micrometer to verify the diameters if you have one.


----------



## jim18655 (Oct 20, 2016)

Any possibility the shaft is bent on the motor?


----------



## Bob Korves (Oct 20, 2016)

Drilling is a roughing operation.  It just removes bulk material.  It does not make a hole to size or locate the hole accurately. To locate a hole accurately requires it to be bored after drilling or otherwise opening up the hole.  Boring is poor at removing lots of material and is poor at meeting a precise hole diameter.  Reamers do not start holes, and do not locate holes accurately.  Done properly, reaming finishes a hole that is round and to size.   The process, then, is to drill the bulk material, bore the hole in the correct location but a bit under size, and then ream the hole for the final dimension and accurate roundness.


----------



## mike sr (Oct 21, 2016)

I was also wondering if it was for a welding turntable, I have built several of these for tig welding, my next one will be with a stepper motor.
I too am curious as to what it will be used for??
I dont see a mention of a center drill to drill a pilot for the drill so that it starts centered in the hole? 
As mentioned in previous posts drill bore then ream and the hole will be straight. Also how the motor shaft is pressed into the plate will make a difference as well, everything should be done squared up in a press as it can press, as it can be a bit crooked as well especially on a steel shaft that small into an aluminum plate of that diameter.


----------



## kingmt01 (Oct 21, 2016)

Personally if I need a center hole 90° too two parallel sides I will drill my center hole & bore it to size. Then I make a mandrel with a center hole on both sides & turn a slight taper on it between centers. I then put a spot of Crazy Glue on the mandrel & press it in the hole. Turning the the mandrel between centers I cut the two surfaces 90° to the center then the outside concentric to the center. A little heat & the mandrel falls out.

ETA: Careful cutting because if you get the part hot cutting the mandrel will come lose.


----------



## prasad (Nov 24, 2016)

mikey said:


> May I suggest that you go on ebay and find a small boring bar? Micro 100 sells some really nice ones that will do this job easily.
> 
> The reason I suggest boring is because a reamer will follow a crooked hole. It will have a nice finish but the hole may not be straight. A boring bar will cut the hole straight AND give you a good finish; how accurate the bore will be depends on your skills when you bore it.



Hi Mikey

I received the Micro 100 boring bar. It is really tiny. However I am not sure how to hold it in my tool post. Is there a dedicated holder to hold it? I searched the Internet and unable to find one. The boring bar I received is "BB 100600" i.e., 0.1 inch minimum hole and 0.6 inch max depth. 

Thanks for your advice
Prasad
Eastern PA


----------



## Wreck™Wreck (Nov 24, 2016)

You make a tool holder, drill then ream a bore through a square or round steel bar, drill and tap some set screw holes then place into the tool post.


----------



## rlgustin (Nov 24, 2016)

Yes a lot of times we of times we make or own special tool holding devices. This is the fun part of what we do.

Sent from my LG-D850 using Tapatalk


----------



## mksj (Nov 24, 2016)

You can also mount the boring bar in a square/rectangular shank with some set screws to lock it in place, then put that in a standard insert holder. I would use a dial/indicator gauge to make sure the platter is running true in both axis when you chuck it up.


----------



## tq60 (Nov 24, 2016)

Start over and change order of operations.

Repeat as before and make front side.

But do not finish cut but get close.

But first use a mallet and tap against the stock as you tighten the jaws and rotate the Chuck and repeat this.

You will hear a different tone when the stock is flat to chuck.

When drilling hole use short drill and 

Now get a bolt that is a very snug fit in your hole and find one the is not threaded where it interfaces with the work

Better would be to thread some stock so it can be placed in the Chuck then simply remove nut to remove disk, this is a mandrel approach.

Tapping against chuck should have made it flat.

Now place on mandrel and take tiny finish cuts to final size.

Flip to clean up back side.

Sent from my SAMSUNG-SGH-I337Z using Tapatalk


----------



## Christian Poulsen (Nov 24, 2016)

Yes as said above by some, and assuming you indicated dead on (.25?!!, even .025?!!)...anyway assuming  you indicted dead on when you flipped the part and the motor shaft is not bent or running out of concentricity or something is going on with that...
...even a tailstock that is trammed in (adjusted) (push/pull for y) and shimmed for Z ) and the part is center drilled nice or the centerdrill hole angle is "kissed" with a toolbit; Will not drill dead on...so boring to size after undersize drilling is the way....
....You can save this part as aluminum is easy to plug...bore your part, lets say 1/2" oversize (with a nice finish)...turn a plug with a nice finish (I like about .001 oversize just eyeballing your boss OD size and hole in the picture but .001 per inch press (dia) is a rule of thumb for soft steels and alum.) ...turn the plug length oversize too (say 1/4" "longer" for some meat to press or pound on)....put a little lead in on one end of the plug and press (or pound the heck out of it) in...be sure to get it started straight on a flat supported set up and use shims or something to make sure the plug goes at least a couple of thousands through past the lead in and once it starts going don't stop until it goes through (antiseize (lube) is also nice to use)
...then indicate the faces of your part and face the prodruding plug ends off nice and indicate all again and center drill and drill undersize and bore to size (don't get it it too hot while remachining as if the part gets too hot it may grow and the plug will loosen')

PS The Turkey is on the smoker and will be done at 1:00...Happy Thanksgiving everybody!


----------



## Christian Poulsen (Nov 24, 2016)

tq60 said:


> Start over and change order of operations.
> 
> Repeat as before and make front side.
> 
> ...


....with all due respect TQ, tapping the finished side against the jaws of a chuck (even a good unworn one) is assuming too much for the opposite side to be machined parallel to it and therefor the hole to be straight too...to do it right, besides indicating any ods/id to each others sides, a test indicator should be "hooked" over to that finished face (chuck side) and tapped in (or "out") to dead on...if'n that back side (face) is out even, just say .002, at around the 6" dia. the hole will be out of "straight" (yada, yada)
...but yes, a mandrel/arbor set up with a decent OD size and "kissed" flat and parallel face is nice too....


----------



## mikey (Nov 24, 2016)

prasad said:


> Hi Mikey
> 
> I received the Micro 100 boring bar. It is really tiny. However I am not sure how to hold it in my tool post. Is there a dedicated holder to hold it? I searched the Internet and unable to find one. The boring bar I received is "BB 100600" i.e., 0.1 inch minimum hole and 0.6 inch max depth.
> 
> ...



As Wreck and the others have said, I would make a tool holder out of square stock. Just plain mild steel keystock from the hardware store will do. There are two ways to do this simple job that I can think of - one would be to put it in your 4JC and drill and ream a 1/8" hole and tap two holes for screws to hold the boring bar and lock that in a standard tool holder; the other would be to use a slitting saw and cut a slot from the side of the square stock into the slot. When you tighten your tool holder screws down onto the boring bar holder it will compress the slot and hold the bar solidly. I would favor the latter approach; I dislike clamping down on small diameter carbide tools - while unlikely, they do crack.

Whichever way you go, I would orient the flat at the tip of the bar so it is horizontal. You can turn it a degree or two to achieve some positive rake if you choose as long as you have enough clearance under the cutting edge. That carbide bar, small as it is, will hold pretty tight tolerances so go slow, measure often and you'll be fine.

Let us know how it goes, Prasad, and a Happy Thanksgiving to all!

EDIT: Sorry Prasad, I forgot to ask if you have a boring bar holder. In that case, make a simple sleeve on the lathe, drill and ream it and slit it down the side. Then stick it in the holder and you're all set.


----------



## rlgustin (Nov 24, 2016)

Some of the best challenges I have ever had was saving a part that was wrong. Take your time make sure your setup is sound and good luck. You've received some very good advice. Happy Thanksgiving.

Sent from my LG-D850 using Tapatalk


----------



## tq60 (Nov 24, 2016)

Christian Poulsen said:


> ....with all due respect TQ, tapping the finished side against the jaws of a chuck (even a good unworn one) is assuming too much for the opposite side to be machined parallel to it and therefor the hole to be straight too...to do it right, besides indicating any ods/id to each others sides, a test indicator should be "hooked" over to that finished face (chuck side) and tapped in (or "out") to dead on...if'n that back side (face) is out even, just say .002, at around the 6" dia. the hole will be out of "straight" (yada, yada)
> ...but yes, a mandrel/arbor set up with a decent OD size and "kissed" flat and parallel face is nice too....


You tap it against the Chuck on the rough cut.

If you wish to dial it in fine but that is for after you have it on the mandrel. 

If the face of the Chuck is such that seating the work against it causes it to be off due to uneven face then the Chuck is not suitable for work.

Sent from my SAMSUNG-SGH-I337Z using Tapatalk


----------



## Christian Poulsen (Nov 24, 2016)

tq60 said:


> You tap it against the Chuck on the rough cut.
> 
> If you wish to dial it in fine but that is for after you have it on the mandrel.
> 
> ...


I hear you TQ but unless your making multiples why ruff?...
Turn and finish the one side ODs and faces with the "boss") (ruff drill and finish bore or wait for the other side (it makes no diff.) ...
...flip and indicate OD and the back finished face and face off to thickness...
done...

....although granted, I have a box of several arbors, some aluminum and some mild steel, with various OD's (face area) with threaded holes, bolts and threaded rod with nuts and "washers" to turn parts..once you have em', you have em' and can revise em' with or without "bosses" to locate finished ID's too whenever/whatever for OD lathe work and OD grinding...


----------



## tq60 (Nov 24, 2016)

Why ruff?

Depends on how picky you are or need to be.

Holding in the mandrel may not hold the part properly for the rough cutting.

Ruff cut may be within 010 or 005 of final then in the op once it is spinning on the shaft or arbor one can remove or clean up any minor stuff.

We do finish operations in same operation if following operations not dependent on it.

If one is making a part that needs to run true on a shaft it can be better to affix to a mandrel to do the last cuts to insure it runs true on that shaft.

Sent from my SAMSUNG-SGH-I337Z using Tapatalk


----------



## Christian Poulsen (Nov 24, 2016)

tq60 said:


> Why ruff?
> 
> Depends on how picky you are or need to be.
> 
> ...


Tis' a simple part...
Picky would be what ever the test indicator says on the OD's and faces on both sides when done (for one part)...
...if you bore an ID to size to the OD (OD's) and the face (faces) dead on, the hole (bore) will be dead on...
...more set ups including to/with an arbor = more chance of error...
...2 set ups for 1 part (besides the OD cutter, face cutter (or turn tool or holder) and change to boring bar)...one side then flip to the other side and indicate = done for one (in this case using shims (pads) or a ring so as not to mar up the boss on the 1st side)...

...for turning mutiples I would still finish the major OD, OD of the boss, face both faces and drill and bore the hole to size all in one set up in the chuck (just by ruff indicating or eyeballing the stock concentric and straight depending on how much xtra stock there is)...then face and turn a nice fit boss on an arbor to all the finished ID bores and slip the parts on one at a time, tighten the bolt (or nut on the threaded rod) with proper sized "washers) and just face them off to thickness (but the 2nd side face on the multiples won't be guaranteed as dead on parallel accurate as what a indicator tells me if I  test indicate the back sides...and I still have to cut the extra of the 2nd side under the bolt/washers unless I counter bore the hole to face the whole 2nd side (unless I use an expandable arbor in the ID's (usually for a bigger ID on bigger OD parts and still with those you have to indicate)
... but yoose' could also tap multiples around to dead on and face them all to OA thickness 1st...and then yada, yada (lol)

...Add: Its just as easy to adjust an OD to .0002 concentric and knock a face around to .0002 or less out of flat/parallel as it is to .002... and maybe takes another, what, 30 seconds or a minute.

...Add: Everybody, besides a 1 or 2 inch dial indicator, needs a .0005 grad  0-15-0 (.030 total travel) test indicator with attachments and a mag base for use in set up at all Machine Tools (except the saws)...
I have a Starret "lost word" (lol), a Brown and "scrap" (lol) and a B&S .0001 all with the various atachments including mag base clamps, collet "do dads" for mills and EDMs, and a mini mag base and a "snake" mag base besides a couple of 1" and 2" dial indicators with bases

Just tightening a center drill or drill in a drill chuck in a lathe tail stock yoose' can stick the mag base on the chuck if a part is in it and sweep the center drill...or drill...or reamer on center to the spindle...same in a drill press...or a mill...
...and yada yada (dozens of other thangs")


----------



## kingmt01 (Dec 1, 2016)

Will the shaft of the motor fit in the lathe between centers?


----------

