Wear comp

[Thad]

When you use wear comp, do program it for a nominal size tool and then make the comp adjustment at the control, or program it for the actual size cutter being used and use a zero comp at the control?

 

All but one of us here program for the nominal size and then comp at the control. For example, if I have a .980 EM, I'll program it using a 1" EM and then comp to -.02 in my tool table. Well, today I had a problem (call the welder). I programmed for a 1" EM but my actual was a .895 resharp. It should have finished at -.105. I started off at -.098 to step it in. Everything looked fine in the machine graphics, but it would've cut a complete circle in my part had I let it run. I think the control got confused with the large comp value and did what it thought it was supposed to do.

 

Yesterday, I had a similar situation and comped to -.113. That worked out just fine. It was a different part and a different cutter. I wonder if the geometry was just right where it confused the control. This is also why I'm been waiting on Jack Mitchell's "theory of CRC" thread.

 

As I mentioned earlier, all but one of our guys program like this. He programs for the actual cutter size and he has never had any trouble. I'm starting to think that is the way to go. That's what I did on this part to fix it.

 

How do you guys do it?

 

Edit: This happened on a Fadal.

 

Thad

[Fred @ Slate Industries]

Full size tool in MC

.000 tool diameter in the control

To size you cut -.001 in the control etc.

 

*Except when you Tap then you must call out the tool in the control or the speeds n feeds wont sync.(You will only do that once)!

[robk]

quote:

---

How do you guys do it?

---

Nominal size tool and then make the comp adjustment at the control. A lot safer way IMO. We run alot of the same programs, and when the tool comes back from regrind there is no need to re-program. Isn't that one reason the control manufacturer offers that option?

[CAM-mando]

Nominal size in MC, comp for regrinds at the machine.

 

The other way around tends to keep the welder busy

[Matthew]

I always program a nominal size tool in the computer and then make adjustments at the machine. But you have to make sure you have enough leadin-leadout if your tool is a lot smaller.

 

quote:

---

As I mentioned earlier, all but one of our guys program like this. He programs for the actual cutter size and he has never had any trouble. I'm starting to think that is the way to go.

---

I would not recommend this. If someone decides to put a 1" cutter in when it's programmed for a .980 cutter you would cut too much material out of the part. If you have it programmed for the 1" and put a .980 cutter in, your part would still have .020 material on each side. All you have to do is make an adjustment and recut, the part is not scrapped.

[Tom Dorgan from American Precision]

Sometimes the Break Arc will cause it to make a full circle on leadin/out arcs. I changed to a setting of 2 and solved this problem on my control. Look in post for this:

 

# --------------------------------------------------------------------------

# General Output Settings

# --------------------------------------------------------------------------

abs_inc : 0 # Absolute or Incremental positioning at top level

# 0 = absolute

# 1 = incremental

sub_level : 1 #Enable automatic subprogram support

breakarcs : 2 #Break arcs, 0 = no, 1 = quadrants, 2 = 180deg. max arcs

[?Mark]

quote:

---

program for the nominal size and then comp at the control

---

That is what I've been doing for years.

Never had any problems, but I don't comp. us much as you do. We almost never regrind flutes, we cut off used up end so it's shorter but dia stays the same.

With specials it's different. I program them to actual dia.

CC is a tricky thing to deal with. If for ex. you do contour and need two paraller walls to be within say .0005" and your E.M goes into a very sharp corner before hitting one of those walls you will be off tolerance if cc of more than .0005" is used.

Wonder if anyone else noticed this problem?

Something I learned years ago to pay attention to.

Regards, Mark

[Storkman]

I program nominal for standard endmills. Specialty tools to actual size. All our machines use radius instead of diameter though. Ex. program 1", tool .980", comp offset -.01".

[Thad]

The error didn't occur during the entry move.

 

For those who comp at the control, do you ever end up using a cutter that is .100 or more smaller? I didn't take the time to check which size actually made it gouge, but .005 would have worked and -.05 didn't.

 

Thad

[Storkman]

quote:

---

do you ever end up using a cutter that is .100 or more smaller?

---

Yea Thad, we do it all the time. We have our own cuttergrind dept. So we use them right down to nothing.

[robk]

quote:

---

For those who comp at the control, do you ever end up using a cutter that is .100 or more smaller?

---

Yes. Actualy I prefer to use re-grinds. The tool rolls around the corners much nicer.

[Storkman]

I have had issues like you encountered, But it had to do with the way the machine interpreted the code. Sometimes if I try to cut a half circle or a whole cicle, it comes out "egg shaped". If I set my post to break arcs at quadrants. It works fine. Nice and round. This only happens on a couple of machines. Try to keep track of that when you have 36 of them.

[chip]

Close tol. bores pockets etc. I program the finish dimension. +.005 Stock... cutter comp on the machine to dial it in. No re-grind here.

[?Mark]

quote:

---

but it would've cut a complete circle

---

Breaking cir. might help as mentioned by tommyd

. Also what might get screwed up on fadal control could work on another control. If you keep having those issues and must use so much regrinded tool it might be good idea to switch to programing an actual size.

Do not trust CC

Kind regards, Mark

[crazy^millman]

We use regrinds here Thad alot for roughing or for one or two part runs of something. I will also use them sometimes for C/B or other thing that are not a tight tolerance to keep tool cost down on a job. Not as small a .1 smaller but have found if you have to make extreme changes when using wear can get unpredictable lead in and lead out at the machine that Mastercam will not show you. .1 is what I consider extreme and like said before give yourself enough lead in and out.

[CAM-mando]

Possibility,

 

If you toolpath geometry with a tool in MC that is larger than an internal corner radius of the contour geometry and then run the program with a smaller tool, you will get a gouge in the corner because the code will be two linear moves that intersect.

[jeff]

I almost always have the comp set to "control"

And program for 1" dia endmills whenever possible.

If the operator used a .460 dia endmill to finish his comp at the machine will be .230 when the part is finished.

I never let them do the math at the control to allow for a comp setting to be say -.01,just half of the cutter dia when to size.

Sooooo much easier and eliminates alot of operator errors.

Also sometimes,when the tolerances are wide open,I'll just program to size and leave the comp setting to "computer".

[jeff]

I almost always have the comp set to "control"

And program for 1" dia endmills whenever possible.

If the operator used a .460 dia endmill to finish his comp at the machine will be .230 when the part is finished.

I never let them do the math at the control to allow for a comp setting to be say -.01,just half of the cutter dia when to size.

Sooooo much easier and eliminates alot of operator errors.

Also sometimes,when the tolerances are wide open,I'll just program to size and leave the comp setting to "computer".

[Thad]

I put the file on the FTP. It's called D84.zip. The red is the newest trim line that I had to cut. I created a purple circle approximately where the tool wanted to cut a circle through the part.

 

I'll check our break arc setting in the post, but won't feel comfortable changing it. It's set the way it is from our reseller since having some unexplained part violations in the past.

 

Jay, if you see this, you can delete the D84.MC9 file from the FTP. I sent the wrong one. The zip file is correct.

 

Thad

[Thad]

-

[?Mark]

I think using tangent instead of perpendicular lead in-out could make a difference. Leave other settings the same and give it a shot.

Hope it works.

Couldn't find a purple cir. on black background at first

Regards, Mark

[Thad]

quote:

---

I think using tangent instead of perpendicular lead in-out could make a difference.

---

One purpose of showing you the file was to show you where the gouge occured. It wasn't at the entry. Even if it was, I wouldn't use a tangent line to turn comp on. That would *guarantee* me unpredictable results.

 

Thad

[?Mark]

quote:

---

I wouldn't use a tangent line to turn comp on.

---

The arc in your case is tangent not the line and the cc is read and adjusted on a first line then makes 90 deg. arc and continues along a geo.

Propably when perpendicular lead in was used there wasn't enough "space" for a machine to adjust cc so it did it on one of the next moves.

I never use perpendicular lead in with tangent arc selected , but maybe I'm wrong.

 

Regards, Mark

[F. JAVIER]

"Propably when perpendicular lead in was used there wasn't enough "space" for a machine to adjust cc so it did it on one of the next moves"

I think you found the problem!!!!

[Maxi]

Are you using R or IJK in your arcoutput?

If you are using R try switching to IJK.