What's new
What's new

Trouble holding size after insert change

metalsurgeon

Plastic
Joined
Jan 4, 2017
I've been working on shaft 'blanks' that get a spline rolled on 3 sections. The journals that get the rolled spline are toleranced +/-.0007". Our machine has been holding the tolerance with devastating accuracy,and I am using a 35 degree inserted diamond for finishing, but seem to be having some consistency issues after changing my dulled finishing Insert. The holder uses a camlock and a secondary clamp. After changing the insert I've been backing off my X wear offset .004" because that's a bit better than the average inconsistency I am seeing after an insert change (ranges between .001"-.0035"). So every 25 parts or so I find myself sneaking back up on the finish size and would appreciate any advice on how I can get better than .0035" size consistency after a insert change.
 
Long answer, you can't. Not to sound so pessimistic but there are so many things that need to line up for an insert to cut the same after an insert change that it would be nearly impossible to do it consistently again and again.
 
Rather than concerning yourself with consistency between insert changes I believe you would be better off looking at ways to reduce the number of times you need to change the finishing insert.

Either adding another pass from the roughing tool to leave less material for the finisher or even better, add a semi finish tool which leaves a small and consistent amount of stock for finishing. Doing these instead could allow the finishing tool to last 2-3 times longer.

Btw, what do you mean by diamond tool, the shape or the actual material of the cutting edge?
 
You didn't mention whether you have a tool setter arm, or maybe you do but can't use it when the part is still in? If you're able to zero the tool on this, it's only a matter of re-entering the X wear offset you had with a sharp tool producing the correct diameter. That should be the same even if your insert isn't exactly the same dimensions.

If you don't have one, or can't use it - well, I was going to say there isn't another easy way.... until the comment about insert tolerance. It could work if you're meticulously clean and consistent mounting the insert.
 
I'm currently leaving .008" to finish, shafts are 58" long, 25 seems to be the average number before the finish starts get that 'fuzzy' texture and I have consistent trouble with the tolerance. I was referring to the insert shape is 35 degree diamond, the insert itself is carbide.
 
Yeah, I'm just trying to figure out a way to help speed up that first part after the insert change, but this is probably one of those situations there's not a quick fix for.
 
Not sure off the top of my head. Not at work so I don't have the box to look at. I will be sure to look in the morning.
 
What is the material and the diameter?

58" long, I bet that takes a while to run. What is the tool nose rad and the feedrate? What is the actual brand and grade of the insert?

Is there a reason why you're using V inserts, to minimize tool pressure?
 
4140 pre hard. The journals finish at 2.7279" using an ingersoll insert with a .031" radius. Using this style insert to finish because the shaft size ramps up and down both sides of the journal from 2.605" with a 30 degree angle on the front and 45 degree angle on the back. I am currently finishing the journal at .009"ipr, but I am currently finishing the whole shaft at one time not just the journals. That may be part of my problem thinking out loud about this. I could use one tool to finish the 3 journals (they are 7.5" long each) and a separate finishing tool to finish the less critical 'clearance' 2.605" diameters in between. they are toleranced at +/-.006", and I finish that diameter at .015"ipr.
 
I'd definitely be getting another tool in there to save your finishing tool for where it matters.

Another thought, since you don't have a tool setter arm, is to set up an indicator somewhere to check the difference after an insert change.

Or, chuck a short piece of stock and take a cut or two before starting on your next actual part. You could make your adjustments here instead of that big expensive part. Of course it might not give exactly the same diameter right near the chuck but you should get an idea of the relative difference so you can calculate a new X wear offset.
 
Depth of cut to nose radius ratio my also be an issue.

but the best idea is to have a second finish tool and use this one where it counts. good idea.
 
A "V" insert has the worst tip height interchangeability of any insert shape due to the shallow angle vee it sits in.
Going to a tighter tolerance insert will help but finding this in a "A" tolerance will be a difficult.
A "G" tolerance insert is +/.001 on the IC, this is a .0066 variation in tip length in the pocket from one insert to another.
"C" shaped inserts are much friendlier.
Bob
 
Not sure im understanding your shape correctly, but could you use a back wards - opposite hand tool and just finish the steps at one end the other way so you can use a more forgiving insert style?
 
A "V" insert has the worst tip height interchangeability of any insert shape due to the shallow angle vee it sits in.
Going to a tighter tolerance insert will help but finding this in a "A" tolerance will be a difficult.
A "G" tolerance insert is +/.001 on the IC, this is a .0066 variation in tip length in the pocket from one insert to another.
"C" shaped inserts are much friendlier.
Bob

What you wrote makes perfect sense, but I have used Sandvik VBMT cermet inserts for general finishing for years and I never see much more than .02mm variation on diameter between changes from the same box.

I know it would be foolish to rely on that, but it has been my experience.
 
I've given up on VNMG's, they just never repeat.. And I haven't found
a single clamp holder for them yet, still that pin and clamp stuff, and I
HATE the pin and clamp thing... Especially having to find 2 wrenches that I've
misplaced instead of just one.


I've swapped over to VCxx's and been much happier. 2 less cutting edges, but
they seem to repeat a lot better.
 
Short answer, yes. however my plan now is to change my machining strategy a bit to have two finishing tools. keeping one to finish the high toleranced journals, and adding one to finish the less critical 2.605" clearance dimension between the journals. I had an 'aha' moment while reading through some of the responses and talking out loud about the issue at hand last night. I think this will double or triple the finish insert life.
 








 
Back
Top