What's new
What's new

21mb Mill overcutting during high speed machining. Parameters to make it better?

dandrummerman21

Stainless
Joined
Feb 5, 2008
Location
MI, USA
Running a part that we have run before. 1/2" endmill, volumill programming about 4500rpm 200ipm, maybe .040" stepover. Gibbscam is programmed to leave .015" stock (I know increasing this is a possible solution, but read on)

The problem area in question is a rounded area about 1.5" diameter on the left side of the part. about 225 degrees of circle, with some other features on the right side. Imagine a circle shape with a 1" wide rectangle sticking out of it on the right

We previously ran this on a 1993 leadwell 760ap with 0m control. This job ran perfectly well on that. The volumill toolpath did not dig in anywhere, so the .015" stock was adequate to let the finish pass clean it up.

Now, that machine is gone, and replaced with a NEW (lol) 1999 Leadwell v40 with 21mb control. The problem is, the machine overcuts on a couple square corners slightly, and overcuts by a bunch around the big circle (I estimate .025, that is to say it cuts past the .015 stock by .010" or so). Same code, same tool.


Now, i CAN repost the code to leave .030 or so of stock, or maybe slow it down. Maybe find the "finish pass" of high speed milling and slow that down by a %. But I'd like this machine to behave while interpolating like the 0 controls do. We still have 4 0m machines of the era and I'd at least like the same code to work the same in this machine too. Even if I have to slow the machine down.


Offhand, I don't know what motors this machine has vs the other one, but I do know that the maximum feedrate was set to 197ipm on the old machine, while the newer v40 is 394ipm (394 rapids vs 787ipm rapids).


So are there parameters I could change to make it behave? I tried turning down 1422 and 1430 to 5000 (they were 10000) but that made no difference. I think if I slowed down further, they might cause the feedrate not to exceed those rates? I believe a setting of 5000 equates to 197ipm if I understood the book right. So if I set them to 4000 the machine wouldn't feed above 160? Still this doesn't "fix" the issue since the 0m machine had no problem going 200ipm around the circle without overcutting.

I also tried changing accell/decel parameters 1620 (was 100, tried 150) and 1622 (was 50, tried 75) but that didn't seem to have an effect.



The 21/210 operators manual mentions using G08, which this machine does not have (illegal g-code). I have an option parameter list for a 21 that does not show the option existing, and another list for 16/18/21 that does show it as existing, but the bit would not turn on, suggesting that G08 is a 16/18 option only. But why does the use of G08 show in the 21 manual? Would a 210 control have it but a 21 wouldn't? (I don't know what the difference between 21 and 210 is)
 
The difference between any 2 digit control model and any 3 digit control model is the 3 digit model is Windows based. Also, G08 is an option for all 16/18 and 21 controls. But you might want to try G05.1 too, which supercedes G08 and G05. G05.1 is the newest version of look ahead. G05.1 Q1 turns it on and G05.1 Q0 turns it off. Adding an R value of 1 through 10, such as G05.1 Q1 R?? lets you choose between roughing and finishing, basically.

Paul
 
#1620 and #1621 are for accell/decel in rapid moves. take a look at #1622 and #1623.

Paul

I did 1622, it was 50, i set it to 75. I have not yet tried a lower value.

1623 is all 0's. The parameter manual says it should be set to 0 except for special cases, otherwise a round circle will not be possible.

"Except for special applications, this parameter must be set
to 0 for all axes. If a value other than 0 is specified, proper
straight lines and arcs cannot be obtained."



I did also try G5.1, again it is not installed so I get an illegal g-code alarm. I see an option bit for that as well, but I did not try to toggle it because I did not see g5.1 in the 21mb operators manual that I was looking at. I assumed it didn't work since it didn't let me turn on G08. I don't know if there's some hardware or software option that isn't installed that is required for the option.


My 1600 parameters are as follows:

N1601 P 00010000
N1602 P 00000000
N1610 A1 P 00000000 A2 P 00000000 A3 P 00000000
N1620 A1 P 100 A2 P 100 A3 P 100
N1621 A1 P 0 A2 P 0 A3 P 0
N1622 A1 P 50 A2 P 50 A3 P 50
N1623 A1 P 0 A2 P 0 A3 P 0
N1624 A1 P 20 A2 P 20 A3 P 20
N1625 A1 P 10 A2 P 10 A3 P 10
N1628 P 0
N1630 P 0
N1631 P 0
N1632 P 0
 
Sounds like you don't have any of those options on your machine. But I think you knew that. My option price list has AICC at $3800. But you would need that if you hope to get anywhere near 200IPM. Ain't going to happen. You can have Fanuc come in and tune the servos for your machine and workpieces. We know shops that do that to get better performance like you are asking for, absent any kind of greater look ahead.

Paul
 
I solved the issue. The parameter 1622 was the issue.

"Time constant of exponential acceleration/deceleration or bell–shaped acceleration/
deceleration after interpolation, or linear aceeleration/deceleration after
interpolation in cutting feed for each axis"

The setting was 50 for each axis, I changed it to 25. That helped a lot. It no longer overcuts by more than .015. It cleans up everywhere with the finish pass.


I think this makes sense, because the 0m control's parameter for this was parameter 529, which was set to 50 on the 0m control.

BUT the old machine was slower, as I said (half the rapid and feedrates). I assume it is the motor which is faster, because the ballscrew pitch looks about the same (is not dramatically different, anyway).

So since this one's max feeds are faster, it kinda makes sense that the amount of time it takes to get up to speed should be quicker, too. And since it is 2x as fast, the time should be 1/2 as much. Or at least it makes sense to me in a general sense lol.
 
Running a part that we have run before. 1/2" endmill, volumill programming about 4500rpm 200ipm, maybe .040" stepover. Gibbscam is programmed to leave .015" stock (I know increasing this is a possible solution, but read on)

The problem area in question is a rounded area about 1.5" diameter on the left side of the part. about 225 degrees of circle, with some other features on the right side. Imagine a circle shape with a 1" wide rectangle sticking out of it on the right

We previously ran this on a 1993 leadwell 760ap with 0m control. This job ran perfectly well on that. The volumill toolpath did not dig in anywhere, so the .015" stock was adequate to let the finish pass clean it up.

Now, that machine is gone, and replaced with a NEW (lol) 1999 Leadwell v40 with 21mb control. The problem is, the machine overcuts on a couple square corners slightly, and overcuts by a bunch around the big circle (I estimate .025, that is to say it cuts past the .015 stock by .010" or so). Same code, same tool.


Now, i CAN repost the code to leave .030 or so of stock, or maybe slow it down. Maybe find the "finish pass" of high speed milling and slow that down by a %. But I'd like this machine to behave while interpolating like the 0 controls do. We still have 4 0m machines of the era and I'd at least like the same code to work the same in this machine too. Even if I have to slow the machine down.


Offhand, I don't know what motors this machine has vs the other one, but I do know that the maximum feedrate was set to 197ipm on the old machine, while the newer v40 is 394ipm (394 rapids vs 787ipm rapids).


So are there parameters I could change to make it behave? I tried turning down 1422 and 1430 to 5000 (they were 10000) but that made no difference. I think if I slowed down further, they might cause the feedrate not to exceed those rates? I believe a setting of 5000 equates to 197ipm if I understood the book right. So if I set them to 4000 the machine wouldn't feed above 160? Still this doesn't "fix" the issue since the 0m machine had no problem going 200ipm around the circle without overcutting.

I also tried changing accell/decel parameters 1620 (was 100, tried 150) and 1622 (was 50, tried 75) but that didn't seem to have an effect.



The 21/210 operators manual mentions using G08, which this machine does not have (illegal g-code). I have an option parameter list for a 21 that does not show the option existing, and another list for 16/18/21 that does show it as existing, but the bit would not turn on, suggesting that G08 is a 16/18 option only. But why does the use of G08 show in the 21 manual? Would a 210 control have it but a 21 wouldn't? (I don't know what the difference between 21 and 210 is)
Hello, would it be possible to get a copy of your parameter(NC, PMC, macros, etc)? We lost our parameters and there is no available backup. (((NEW (lol) 1999 Leadwell v40 with 21mb control))).
If you can please send it to [email protected]
Thank you
 








 
Back
Top