OD groove out of round

tsabo · Jun 7, 2021

Hey everyone.

I'm machining 420SS on my 1994 mazak qt15n. The part OD is 1.5" and groove OD is 1.257" (+-.001). The groove is about .8" in front of my jaws.

The groove is measuring 1.256 one way and 1.258 measuring 90 degrees from the previous.

I'm using a kennametal top notch NG3189-K 5010 tool. The groove width is .189", so I'm going full width and depth no peck. I'm running 500 sfm at .008" feed/rev. Reducing to .006" feed/rev didn't seem to help. I'm using those feeds and speeds because the finish is good with no chatter.

Every once in a while it seems like i get a part that is within .001" round. I'm not sure where to go from here.

Any thoughts?

-Tyler

TeachMePlease · Jun 7, 2021

You give it a dwell at the bottom of the groove, for at least a couple revolutions?

Gobo · Jun 7, 2021

TeachMePlease said:
You give it a dwell at the bottom of the groove, for at least a couple revolutions?

You are absolutely correct. Seen this may times. It is a parameter setting. I don't recall if that early of the Mazak controls have a TPC setting or not. If so, that is where I would make the adjustment.

Trueturning · Jun 7, 2021

tsabo said:
Hey everyone.

I'm machining 420SS on my 1994 mazak qt15n. The part OD is 1.5" and groove OD is 1.257" (+-.001). The groove is about .8" in front of my jaws.

The groove is measuring 1.256 one way and 1.258 measuring 90 degrees from the previous.

I'm using a kennametal top notch NG3189-K 5010 tool. The groove width is .189", so I'm going full width and depth no peck. I'm running 500 sfm at .008" feed/rev. Reducing to .006" feed/rev didn't seem to help. I'm using those feeds and speeds because the finish is good with no chatter.

Every once in a while it seems like i get a part that is within .001" round. I'm not sure where to go from here.

Any thoughts?

-Tyler

Allow material for a finish pass. Also if you are having problems allow a additional finish pass and check it before finishing. Too whenever you cut corners on processes this is what happens. Many people will also back off the rough and finish and check concentricity preventing scrap. Checking accuracy properly will generally prevent scrapping a first part if one wishes to be careful.

tsabo · Jun 7, 2021

It's a T32B control. I have a TPS button, but I don't think that is what you are meaning.

I did a quick search and it looks like parameter p24 is dwelling at the end of a groove. Mine is set for 3 revs.

tsabo · Jun 7, 2021

Trueturning,

I just tested out a part with a finishing and semi finishing pass. I'm leaving .020" (diameter) on each pass and slowed the feed down to .004"/rev. I am measuring about .0009" to .0011" difference now. Definitely an improvement, but still a wide range.

Would you leave less on the finishing passes? The groove bottom looks to have very slight chatter marks now.

DDoug · Jun 7, 2021

tsabo said:
Trueturning,

I just tested out a part with a finishing and semi finishing pass. I'm leaving .020" (diameter) on each pass and slowed the feed down to .004"/rev. I am measuring about .0009" to .0011" difference now. Definitely an improvement, but still a wide range.

Would you leave less on the finishing passes? The groove bottom looks to have very slight chatter marks now.

I'm wondering if you work hardened it on the roughing pass.

camhead420 · Jun 7, 2021

Try running two passes, but leave nothing for the second, like a spring pass on a small boring bar. If your not getting chatter add a couple more spins to the dwell.

camhead420 · Jun 7, 2021

I see you are getting chatter. cancel that last thought.

Gobo · Jun 7, 2021

tsabo said:
It's a T32B control. I have a TPS button, but I don't think that is what you are meaning.

I did a quick search and it looks like parameter p24 is dwelling at the end of a groove. Mine is set for 3 revs.

Sorry, I meant TPC not TPS. TPC=temporary parameter change. Using this, you can set how many rotations the tool dwells at the bottom of the groove. Sometimes just slowing down your feed rate will solve the problem, but it may initiate chatter.

tsabo · Jun 7, 2021

Yes. The chatter is very slight. I figure the dwells would be almost like spring passes anyways.

digger doug - I figured my roughing feed was high enough to get in and out quick without work hardening, but the sfm might be a tad high. I could be doing it wrong, too, as I never turned 420ss and don't have a whole lot of lathe experience. This is my first time grooving.

Gobo · Jun 7, 2021

Gobo said:
Sorry, I meant TPC not TPS. TPC=temporary parameter change. Using this, you can set how many rotations the tool dwells at the bottom of the groove. Sometimes just slowing down your feed rate will solve the problem, but it may initiate chatter.

Now I see you have your dwell set at 3 revolutions. That should be okay. Any more and you will probably get worse chatter.

CarbideBob · Jun 7, 2021

If one thinks about the machine making helix cut.
If it pulls out too fast the helix of your infeed is the groove surface.
So one needs a dwell or G04, sit there too long if a hard push and you get may get chatter.
Why does that happen? Is the top or bottom of the chatter size to the machine and tool?
The same run problem occurs when making center holes. Bing bang, done and then.....downstream.
.006 per rev with a instant machine pullout should leave you out of round a lot as in .006. Think about it.
Bob

kevin66 · Jun 7, 2021

I would check a finished part with a test indicator before removing it from the jaws.If its too short of a dwell it will show up pretty easy.

tsabo · Jun 7, 2021

digger doug said:
I'm wondering if you work hardened it on the roughing pass.

I forgot that I was testing grooves on a piece of steel before trying the 420ss. I went and checked those grooves for roundness and measured .001"-.002" out just like I'm getting on this stainless. I think it's more than a work hardening issue.

Delw · Jun 7, 2021

tsabo said:
Hey everyone.

I'm machining 420SS on my 1994 mazak qt15n. The part OD is 1.5" and groove OD is 1.257" (+-.001). The groove is about .8" in front of my jaws.

The groove is measuring 1.256 one way and 1.258 measuring 90 degrees from the previous.

I'm using a kennametal top notch NG3189-K 5010 tool. The groove width is .189", so I'm going full width and depth no peck. I'm running 500 sfm at .008" feed/rev. Reducing to .006" feed/rev didn't seem to help. I'm using those feeds and speeds because the finish is good with no chatter.

Every once in a while it seems like i get a part that is within .001" round. I'm not sure where to go from here.

Any thoughts?

-Tyler

A host of things could be causing this. these are the obvious, and most often over looked.
1st jaw pressure and are your jaws Cut round? if you dont use a round spinder your jaws wont cut round did you check the jaws with an indicator.

tsabo · Jun 7, 2021

Delw said:
A host of things could be causing this. these are the obvious, and most often over looked.
1st jaw pressure and are your jaws Cut round? if you dont use a round spinder your jaws wont cut round did you check the jaws with an indicator.

I am using hard jaws. I'm feeding a 1 ft bar through the spindle. The bar fits the liner good. I've tried 175-300 psi on the chuck pressure. This is a 1st op.

The OD of the part is measuring round and so is the stepped feature at the front of the part.

Gobo · Jun 7, 2021

Mazatrol program?

tsabo · Jun 7, 2021

Gobo said:
Mazatrol program?

Yes mazatrol program.

Gobo · Jun 7, 2021

Are you using a "0" grooving cycle? I am not sure if it dwells with a 0 cycle. Put a really crazy number in your dwell parameter and see if it does dwell. If not, you will have to use a "1" cycle or write a Mazatrol manual unit.

OD groove out of round

Plastic

Diamond

Titanium

Diamond

Plastic

Plastic

Diamond

Cast Iron

Cast Iron

Titanium

Plastic

Titanium

Diamond

Aluminum

Plastic

Stainless

Plastic

Titanium

Plastic

Titanium

Similar threads