Help with IJK Rads

[gcode]

Lee,

When you edit your machine definition, are you using the Edit button in the OPs Manager

or the Machine Def dropdown from the menus at the top of the screen.

I ask because the "Min Distance between arc endpoints" tolerance setting is still .0005

in the files you sent me.

It should be .002 or higher.

 

If you edit the maniche def from the ops manager

that edit applies to that machine group only.

To edit the machine def permanently, you need to do it from the Settings/ Machine Derfinition Manager.

 

I regened and posted the file you sent and could see nothing wrong with the output.

I also did it with a new mpmaster x2 post and the gcode was identical

[Gilberto]

edit the post variable "arccheck" in V9 is the same as changing the values on Machine/Control definition in X2.

[Lee.]

G-Code,

 

I edited it from the Machine Def, then went into control def from there, just checked it and all is fine, 0.002

 

Any idea as to what is going on?

[gcode]

I posted your file with your post and a new mpmaster. The code was identical and I could see no problems or tiny arc moves.

I emailed it to you last night. Have you tried running it on your machine?

 

I noticed you are running your filter at the 2-1 ratio. Have you tried changing it to 1-1??

 

I also tried to find numbers similar to the ones you put up here on the forum, but couldn't. Were those the same toolpaths that were giving you trouble?

[Lee.]

My spam filter caught it, I just retreived it.

 

I ran the same file from V9 and it ran fine, maybe I'll compare the two and see whats up.

 

Lee.

[Lee.]

G-Code,

 

Just posted with X2 again after opening the program, fresh start, the NC file now has R - radii instead of IJK.

 

I'm about to blow my mind on this.

 

Help!!!!

[Bruce Kanzelmeyer]

Lee,

 

Look at your V9 System configuration/NC Settings/Filter Settings and adjust your Control Definition/Tolerances settings in X2 to the same values and perhaps your post will then output G code that is same as what you got w/V9...Just a thought.

[gcode]

You have to edit the machine def from

the Settings/Machine Def dropdown and the top of the screen. This permanently edits the machine def

 

If you edit it from the Ops Manager, the edits only apply to THTA Machine group in THAT file only.

The hard drive copy remains unchanged.

[Lee.]

G- thats what I have been doing.

 

I never have changed anything from Ops manager.

 

Lee.

 

I sent you an e-mail

[gcode]

I'm at my day job now.. it may be a while till I can reply

[Lee.]

G,

 

No worries, i'm using 9 til we can get it sorted.

 

Thanks, Lee

[gcode]

check your email

[Lee.]

so, I changed the NC tolerance to 0.001 and it seemed to have fixed the problem.

 

Thankyou to all who helped me with this.

 

I couldn't have figured it out on my own.

 

Lee.

[Lee.]

So, here we are again.

 

I just screwed up another fine job.

 

I am still finding that the difference between start points is too small.

 

I am pasting some code here in the hope that someone can point me to the source of the problem.

 

N1340 G02 X-2.2872 Y-.039 I-.007 J-.03

N1342 X-2.288 Y-.043 I-.0308 J0.

N1344 X-2.2847 Y-.164 I-2.202 J-.121<<<<<<<

N1346 X-2.284 Y-.175 I-2.2053 J0.<<<<<<<<<

N1348 X-2.323 Y-.1938 I-.039 J.031

 

There is too small of a difference between the start points on the lines with the arrows.

 

I've looked everywhere I can think in an effort to greaten the tolerance.

 

Thanks in Advance,

 

Lee

[Lee.]

Bump.

[Hardmill]

Just jumping in here Lee, I see your running a Fanuc

control. The code looks fine, I guessing you need to loosen up

the arc tolerance in your control. I believe on the 16im its parameter 3410

 

Check your manual and loosen it up, that should solve your problems.

 

 

PEACE

[Lee.]

Hardmill,

 

I'm using a Fanuc OM-A.

 

Does this control have settings for this also?

 

Thanks for any help.

 

Lee.

[Hardmill]

Look at your manual, my guess is all controls have it.

 

 

PEACE

[Lee.]

Hardmill,

 

I just ran the same program, posted from V9MR0105

with no problems.

 

It's driving my !@#$%^*&^ nuts.

[Hardmill]

Can you post the code from the same section for both posts ??

 

 

PEACE

[Greg Williams]

Lee,

 

Something must be different can you post both good and bad here

[Lee.]

This is the V9 code.

 

N1350 G01 Z1. F40.

N1352 G00 X-3.2302 Y.0122

N1354 G01 Z-.1

N1356 G03 X-3.0037 Y-1.2599 I3.4188 J-.0475 F200.

N1358 X-2.3344 Y-2.3332 I3.0931 J1.1833

N1360 X-1.0457 Y-3.1802 I2.3543 J2.1781

N1362 X1.229 Y-3.1093 I1.0455 J2.9828

N1364 X2.5786 Y-2.038 I-1.283 J3.0022

N1366 X3.2277 Y.1056 I-2.7468 J2.0018

N1368 X2.8446 Y1.5385 I-3.3727 J-.1342

N1370 X1.9766 Y2.5917 I-2.9079 J-1.5122

N1372 X.0919 Y3.2849 I-1.9808 J-2.4766

N1374 X-1.7321 Y2.7683 I-.0845 J-3.1797

N1376 X-3.0064 Y1.1795 I1.8244 J-2.7688

N1378 G01 X-3.0065 Y1.1793

N1380 G03 X-3.0729 Y.9888 I2.3014 J-.9084

N1382 G01 X-3.073 Y.9884

 

and this is the X2 code

 

N1328 G00 X-2.9243 Y-.5888 Z1.

N1330 X-2.994 Y-.3991

N1332 G01 Z-.1 F40.

N1334 G02 X-3.0177 Y-.058 I2.443 J.341 F200.

N1336 X-3.01 Y.131 I2.4667 J0.

N1338 X-2.984 Y.1465 I.026 J-.014

N1340 X-2.965 Y.14 I0. J-.0295

N1342 G03 X-2.498 Y-.0332 I.467 J.543

N1344 X-2.311 Y-.009 I0. J.7162

N1346 G02 X-2.2872 Y-.039 I-.007 J-.03

N1348 X-2.288 Y-.043 I-.0308 J0.

N1350 X-2.2847 Y-.164 I-2.202 J-.121

N1352 X-2.284 Y-.175 I-2.2053 J0.

N1354 X-2.323 Y-.1938 I-.039 J.031

N1356 X-2.344 Y-.189 I0. J.0498

N1358 G03 X-2.436 Y-.183 I-.092 J-.699

N1360 X-2.948 Y-.404 I0. J-.705

N1362 G02 X-2.969 Y-.4127 I-.021 J.021

N1364 X-2.994 Y-.399 I0. J.0297

 

In the X2 code the problem arises at line 1352 as far as I can see there is not enough difference between X values, this is what G-Code explained to me, so my control doesn't know what to do.

 

Any ideas guys.

 

Thanks, Lee.

[Hardmill]

quote:

---

so my control doesn't know what to do.

---

Thats why Im saying its an arc tolerance issue.

 

Since the code is so different I take it its not from the same

contour in the program, correct ??

 

 

PEACE

[Lee.]

It's the same style of toolpath and on the same part, with the same settings.

 

Not sure why the code is different.

 

I guess thats the point.

 

I'm wondering why it would be a control issue after the V9 code ran seemlessly.

[Hardmill]

Mail Lee

 

 

PEACE