Scrap after Insert Change

Hello all,

I'm looking for any creative ideas or paths for the following problem on a Mori Seiki CNC lathe (NLX 2000).

We are using a certain insert (GRIP 6030Y) which has a tool life of ~30 minutes for our application thus this insert is frequently changed. We've noticed that every time this insert is changed we scrap a part or few trying to get the part back in size and this scrap is really adding up.

We are concerned with three features; the ID size (X offset), Race location (Z offset), and Radius of the ID (R comp). All three of these characteristics are defined by this one tool. We try not change the R comp. unless necessary as the machine has a happy place for it given that our tolerance for the radius is +/- .001." Also, the tolerance for the ID and race location are +/- .00025" and +/- .001," respectively. Additionally, the parts are copper plated adding a whole other dimension of variation due to changing copper thickness from part to part. Although, for this problem lets assume the variation is negligible as we working with our vendor to solve this.

At the moment, we are working to develop a procedure to back off the X and Z offsets every time the insert is changed and then slowly come in. This will certainly help but one scrap part is certainly guaranteed as re-machining the ID several times seems to throw the radius out of tolerance.

Surely that one scrap could be better than our current situation but are there any other possible solutions to this problem or improvements for our procedure? FYI I'm somewhat new to the CNC world so anything help!

Thanks!!

You need to validate the tool's X and Z offsets each time you swap the insert. How you do this is up to you. You can run a different program, on a piece of similar but not precious stock, that cuts a predetermined Z and X, then measure and adjust offsets. Or you can invest in a toolsetter if available for your machine.

Regards.

Mike

Are you using a rougher and a finisher?

When I'm running tight tolerances, my game plan is to dial it in ONCE. Run the
finish insert so that it lasts to the end of the job, or end of the day, kind of
like the old swiss machines, set the feeds and speeds so that it lasts 24 hours.

Make up the time on the rougher. If the rougher varies a thou or 2, 99% of the time
its not going to matter.

If you are limited to a single tool, try backing your speed down 10 or 20%, most of
the time there is *speed* where tool life falls off drastically, and conversely increases
massively. Yes... You will be running slower, but you won't be running scrap parts
(and scrap costs $$$$ not just time) and diddle farting around dialing the part in
AGAIN every half hour.

what amount of tolerance are you trying to hold?

Index the insert, back off 1x or 2x the amount of stock you leave for finishing.Then run the finish pass, measure and compensate.
If it's a production job, you could make up some dummy blanks to dial the fresh insert in on. Size wouldn't matter (usually) as long as it cuts to the programmed dimension. But the key is to dial it in by cutting the same depth of cut as your main program does for finishing.

I use GRIP style inserts often. The torque that the insert is held makes a big difference on height of the insert.
Maybe that is an issue? Have a look in your Iscar catalogue, it does give guidelines for this.

Ok wait, I just saw your tolerances. I agree with the other folks, either dial it in after every change or run a dedicated finisher.
Maybe a thinner rougher and then the finisher.

Guess I would have a break-in program to run 3 parts at the safe numbers then one to sneak up on size.

michiganbuck said:

Guess I would have a break-in program to run 3 parts at the safe numbers then one to sneak up on size.

Click to expand...

I HATE that phrase.. "Sneak up on it". When I first got into this game, I tried that. Smaller and
smaller cuts to "sneak up" on the size I needed.. Didn't work so well.

My method now. 2 nearly identical finish passes. Lets say I'm trying to hit .9995 ± .0005..
Lets say I'm planning on a .025" finish pass (D). I like going in chunks of .025, less chance
of making a brain fart on the micrometer. I'll rough to 1.050", then take my finish #1 at 1.0245"
and measure.. Then offset.. and run the final finish pass.

You'll nail it first time, every time with 2 nearly identical cuts.

To the OP, maybe have 2 programs, one that runs the whole part, and one that takes a
test finish pass, and pauses so you can measure.. Maybe an M0 and a block skip
would work also if you are running a single tool.

I use this method when I'm setting up a part, and I also sometimes use it 100% when its
an expensive part with a lot of other work in it, or the material is fricken expensive.

Have you tried to "map" the error and correction needed everytime you make this change?
Is this amount off somewhat consistent enough to give a good guess at where to go?
Do not just do gut feel off of these numbers happening, chart them.

Option two is a easily measured in machine precut at tool change to point you in the correct direction.
Option there is tool probing.
Option four is higher precision tools and holders or measuring the new cutting tools themselves to a tenth.

If there is any flank weld indexing this type tool can cause big problems. Is there a end one and end two problem simply going back to what end one wanted at the start?
That worn tip one to tip two vs the next new tool may screw up your thinking as to a offset and make it seem all over the place. You will see this in above asked for chart so label ends.
Holder design matters here.

Cut over and sneak up on it works for part number one but as you have seen part two will likely be scrap with these offsets.
On my grinders when this rerun to size is done there is "learned" change in offsets for part number two.

The "+/- .00025" and first part good is a real and big problem. While nice in batch these cutting tools not made to approaching that tolerance.
Many live with one scrap as expected, others have a higher dollar part at this point and put more money or effort in not making a scrap one.
Bob

Any kind of better longer lasting tool you could use for finishing, maybe CBN or diamond ? Also a stronger holder would surely help with flexing.
Pretty sure one of those will cut copper good if its the right grind/edge.

SND said:

Any kind of better longer lasting tool you could use for finishing, maybe CBN or diamond ? Also a stronger holder would surely help with flexing.
Pretty sure one of those will cut copper good if its the right grind/edge.

Click to expand...

.00025 needed. .0001 per side or better.
Buying tools in this tolerance in CBN or diamond? I doubt this.
Add tool into holder, do you own a 20-50 millionths repeatable holder over many runs?

Bob

Bobw said:

My method now. 2 nearly identical finish passes.

Click to expand...

This is good advice. I operate the same way. On manual lathe I make two careful finish passes the same size, measuring in between and make slight adjustment if needed for final cut.

On CNC I usually back the tool off the same amount as finish pass. Run the whole thing, measure it and then run the finish pass again right to size.

You left out the most important factor. What do the blanks cost ?

If it's $3, then the cheapest and fastest way is to scrap one. Run the part, measure, adjust offsets, only takes one part and it's guaranteed. And quick. Plus anyone can do it.

If the blanks run $15 $20 or something, that's a different story.

Bobw said:

I HATE that phrase.. "Sneak up on it". When I first got into this game, I tried that. Smaller and
smaller cuts to "sneak up" on the size I needed.. Didn't work so well.

My method now. 2 nearly identical finish passes. Lets say I'm trying to hit .9995 ± .0005..
Lets say I'm planning on a .025" finish pass (D). I like going in chunks of .025, less chance
of making a brain fart on the micrometer. I'll rough to 1.050", then take my finish #1 at 1.0245"
and measure.. Then offset.. and run the final finish pass.

You'll nail it first time, every time with 2 nearly identical cuts.

To the OP, maybe have 2 programs, one that runs the whole part, and one that takes a
test finish pass, and pauses so you can measure.. Maybe an M0 and a block skip
would work also if you are running a single tool.

I use this method when I'm setting up a part, and I also sometimes use it 100% when its
an expensive part with a lot of other work in it, or the material is fricken expensive.

Click to expand...

First and foremost, thank you everyone for your responses. As a beginner in this trade it means alot as it's easy to overlook many of the simple strategies you have all thrown out.

I'm planning on implementing Bob's idea above as it shows much potential. Along with this we will consider and make use of many of the other ideas suggested as well.

Thanks again! Now, I've got some work to do!

Maybe it's time to try a different tool. The GRIP 6030Y has a +/-.004 tolerance on tool length repeatability. The radius has a +/-.002 tolerance. There's nothing wrong with that and it doesn't mean Iscar makes a bad tool. Iscar may have something available with a better tolerance. Get a rep in and have them go over your application. If they can't solve it then try someone else (ph Horn)

The cost in productivity and scrap lost trying to get the part back in size would likely pay for a more expensive insert that has better tolerance.

Mtndew said:

Index the insert, back off 1x or 2x the amount of stock you leave for finishing.Then run the finish pass, measure and compensate.
If it's a production job, you could make up some dummy blanks to dial the fresh insert in on. Size wouldn't matter (usually) as long as it cuts to the programmed dimension. But the key is to dial it in by cutting the same depth of cut as your main program does for finishing.

Click to expand...

This is what I always have our guys do. The key is always having the same tool pressure. If using a rougher back that up the same amount. Most times I use 2 finish passes just to ensure the tool pressure for the last pass is always the same.

Does not a second pass take more time?
Guessing these not parts where pennies count in the win/lose of a contract?
No way you make a second pass on a auto axle in it's volumes. You nail the two tenths.
Auto pistons tighter.
Bob