What's new
What's new

Turned part and concentricity issue

Corn

Aluminum
Joined
Nov 3, 2019
Hi,

I'm baffled and can't understand how following is possible. I've tried to make slitting saw holder for use in ER25 collet chuck, but no matter how I do it there is ~0.15mm concentricity error which is alot. First of all the part is like this:
slitting_saw_holder.jpg

I've actually tried three times to do this and every time I get the same error. First time I turned it in two different grips on 4 jaw chuck. It was properly indicated to run true before starting to machine the other end. When installed to ER25 collet chuck with 0.08 AA collets it had runout of ~0.15mm

Second time I machined it with one grip. In the picture chuck end was on left side and all three diameters were turned on one grip. Got the same error when attached to collet chuck.

Third time on precision Bison 3 jaw scroll chuck and with one grip. This time so that the 25mm stock was around 55mm extended from chuck and supported from other end by the tailstock. First turned the biggest diameter to 24mm then the 16mm diameter for the slitting disk. Then 15mm diameter for the collet. Next drilled the hole and threaded M8. At this point I indicated the slitting disk shoulder and it had 0.01mm runout. Last I parted it off. Put it in the ER collet and again ~0.15mm runout! :mad5: Btw. that 15mm diameter was turned with parting tool in last two cases. Lathe is Harrison M450. Material 17-4PH.

I've tried in two different milling machines and two different collet chucks and collets. Still the same. This is driving me nuts. What in earth is going wrong?

Your help is greatly appreciated.
 
You tried two different milling machines and collet chucks but didn't measure the actual collet chuck runout?
Thats where I would start, get yourself something like ground 15mm shaft and check the runout of milling machine chucks.
 
There are very elusive grimlins at work any time you make a slitting saw arbor. ANY time. To get a concentric holder, leave stock one the saw's locating diameter. Grip a tool holder in your milling vise so that you can TURN the locating diameter as well as FACE the shoulder. The grimlins are not quick enough to mess up both operations.
 
Three times and always bad? Your second time seems to have been bullet proof. I am suspecting the collet or collet chuck OR the spindle you are putting them on.

This seems like one where you have to check things one step at a time.

For a quick check, I would find a 15mm rod and chuck it in one or both of those collet/chuck combos and see what the run out is. Could be some chips in the mounting of the collet chucks or some other problem there. Drill rod is fairly round and straight so the shank of an undamaged drill bit would do for this.

Your parts have three round, cylindrical parts. You could check them on a surface plate using the largest diameter as a reference. First check that larger diameter by taking several readings with a micrometer at various rotations. They should all match within tenths. Then check the two smaller diameters height off the plate as you rotate them to different points on that larger diameter. Those readings should all match. If they do, then the parts are probably OK. If not, then you can look further in your methods of machining it. This test should point you in the right direction: making the parts or the collets/chucks/spindle where they are to be used.
 
Three strikes and out.
All tries doing different show the same error? That should never happen.
Trust level of the measuring the finish part, could there be anything there?
This is a big error, something smells not right.
Bob
 
Curious how you measured the runout? Sometimes an indicator will have some backlash on a rack and stick a bit, such that it jumps around a bit. That's one possible explanation for getting the same bad TIR readings.

For starters, I'd try measuring runout with the part still in the lathe. You might have better control of indicator location and be better able to see what's going on. If it's good there, then it's on to checking your milling spindle, collets, etc.
 
As others have already stated, it is nearly impossible to have that much runout on a part that size turned in a single operation. Depending upon the condition of the spindle bearings you may have some lobing, but probably to little to measure.

That leaves 4 potential problems

1: As stated earlier, maybe the collet / holder is bad, or there is a chip inside the collet pushing the part to one side. Put an endmill in it and see if the runout is still there.

2: Wrong size collet. You should use a 14-15mm collet for a 15mm shank. if you are using a 15-16mm collet and closing it all the way down, this will likely cause runout.

3: Maybe the shank has some taper in it. 0.003" (0.075mm) taper in the shank would cause about 0.006" (0.15mm)TIR

4: No gap between the part and collet nut. This would be my bet, try and leave a gap between the turned shoulder and collet nut. The collet nut will not be square, and because tightening an er collet pulls the part downward ~0.3mm, it will cause significant runout. Leaving a gap will also alleviate problems with a radius in the corner of the turned part.
 
Allowing nice finish cuts on the od’s? Or is it leaving od distortions from heavy cuts. It only takes a little. I agree checking it in the lathe before partoff is wise. Then when machining the boss on the end before cutting I would see if that runs true to od and then after turning on the face of the part.

It could be the collet or perhaps a unseen chip or where a chip boogered up the collet and then fell off. One could dykem the collet and clamp a solid pin and look for the dykem to wear off and that may show up a dingie doo.

Check collet first.
 
Any chance you might run the part between centers.

about .006 is a lot of error
What runs out to what? the bore hole to the OD? or one diameter to another? for a turn all diameters and the part-off I used to tool bit spot my hole so any error in the start of my drill or center drill could not cause part error.
Very often for near zero jobs I would run the part diameters between dead centers. the head center turned at the time of running the part.
I never ran a really good lathe so had to work around machine errors to do .005 / .001 or so work down to a part spec that needed near zero.
 
There are very elusive grimlins at work any time you make a slitting saw arbor. ANY time. To get a concentric holder, leave stock one the saw's locating diameter. Grip a tool holder in your milling vise so that you can TURN the locating diameter as well as FACE the shoulder. The grimlins are not quick enough to mess up both operations.


This man speaks truth,,one of those things
 
that runout actually might not be so bad, maybe just enough to correct the runout of the saw?
 
Agree with you, if the whole part was sticking out and you turned 3 diameters, then parted it off all should run dead true...Might you check it in a v block for error?

If that checks good the holding collet may be blame as ThebigLeblosky mentioned.
 
Got my sanity back... That holder is darn near perfect when measured. Collet chuck seems to be battered and both 15mm collets are well, not so true. That makes me wonder is it harder to make collets from the top end of clamping range than say mid range? Good point also to leave gap between the nut and shoulder. Never thought about that. Thank you all.

If I may continue off topic. Is there any way to heat treatment Condition A 17-4PH to H900 condition without sophisticated equipment? If I correctly understood it would need 900F / 482C for one hour and let air cool to room temperature. Kitchen oven doesn't quite reach that far...
 
You can make a holder for your mill, if the mill is to be used and in one machine only. bore the 15mm hole with the holder in the machine. With having a line up mark on your holder and on the mill spindle it will run near spot on.

Turn one of the others to .500 and use it in a half inch end mill holder.
 
If the run out is seen when using the saw - its only cutting on part of the saw blade - its the saw. If its going crunch crunch crunch you can help it with a deeper cut and smooth definite feed to keep it cutting more all around.

Only way around this would be to sharpen the saw on the mandrel.

And a light wring fit of blade to arbor helps too.
 
I have made quite a few arbors for slitting saws. Even though the arbors run dead true you may find that the saw seems to give you an intermittent cut. These are not cheap saws either. I have never really been able to figure it out so I just live with it.
 
Yes, those slitting saws are another story. I have half a dozen of them and all seem to have concentricity issues...
 








 
Back
Top