G code problem

[Guest]

I have a problem this morning I have not encontered previously.

 

I have a contour that I have chained in X below

 

quote:

---

G00 G90 G54 X-.1207 Y-.0434 S12000 M03

G43 H9 Z4. M08

Z.87

G01 Z.48 F8.

G41 D9 X-.1571 Y-.0069 F5.

G03 X-.1936 Y.0081 I-.0364 J-.0364

G01 X-.257

X-.2611 Y.0071 <-------

X-.2641 Y.0041 <-------

X-.2652 Y0. <-------

X-.2641 Y-.0041 <-------

X-.2611 Y-.0071 <-------

X-.257 Y-.0081 <-------

G03 I0. J-.0081

G01 X-.1936

G03 X-.1571 Y.0069 I0. J.0515

G01 G40 X-.1207 Y.0434

G00 Z4.

---

This is the same exact contour done in V9

 

quote:

---

G00 G90 G54 X-.1207 Y-.0434 S12000 M03

G43 H9 Z4. M08

Z.87

G01 Z.48 F8.

G41 D9 X-.1571 Y-.0069 F5.

G03 X-.1936 Y.0082 I-.0364 J-.0364

G01 X-.257

G03 Y-.0082 I0. J-.0082

G01 X-.1936

G03 X-.1571 Y.0069 I0. J.0515

G01 G40 X-.1207 Y.0434

G00 Z4.

---

Notice in the X post where the arrows point all of the extraneous code.

 

Has anyone seen a problem like this?

 

Any suggestions on what might be going on?

[gcode]

I had a similar problem with a Haas post. I went

to the Machine Definition and changed

the "General Math fucntion tolerance" from

.0001 to .00005 and it fixed the problem.

I sent a report in on this, but have not recieved

a reply yet

[Guest]

Nope, that didn't work.

 

Thanks gcode

[gcode]

Did you Regen after you changed the setting??

also try setting arcs to break at quadrants

[gti_jay]

Try the "FILTER" option in the contour parameters window.

 

Be sure create arcs in XY is selected

[Guest]

gcode,

 

I tried the "arc to break at quadrants" and that seemed to do the trick.

 

Just kind of funny that something I have done all the time now causes me to change my settings, but hey it worked.

 

Thanks

 

gti_jay,

 

Thanks for the suggestion

 

[ 10-17-2005, 01:01 PM: Message edited by: jmparis ]

[P_Scott]

jmparis,

 

Glad to see you found a solution John. How're you doin'? Hope you didn't get flooded out like so many others in our state. My advice would've closely resembled gti_jay's. That's what it looked like to me. Possible breakup of a spline into many linear moves. Check your geometry. Is there a spline instead of an arc at the location of these lines of code? Splines can often be confused with arcs or even straight lines. The only way to be certain is to analyze the entities and find out what they are. Or you could attempt to Edit/Simplify (Modify-Convert to Arcs in V9) and select All - Entity menu - Splines. If anything highlights, you've got splines. HTH

[Guest]

Peter,

 

Nope no splines, just edge curves.

 

No problems with water up around me, I live on a hill

 

I'll see you next week anyway, I'm in for the Advanced class.

[Guest]

Actually, no this did not solve that problem. I just read the code a little closer, it seems there is a G01 missing after a G03 move

 

quote:

---

G01 Z.48 F8.

G41 D9 X-.1571 Y-.0069 F5.

G03 X-.1936 Y.0081 I-.0364 J-.0364

G01 X-.257

G03 X-.2652 Y0. I0. J-.0081

X-.257 Y-.0081 I.0081 J0.

X-.1936 <------------should be a G01

G03 X-.1571 Y.0069 I0. J.0515

G01 G40 X-.1207 Y.0434

G00 Z4.

---

 

I placed the file in the MCX folder named

JMP_CONTOUR_PROB.mcx

if anyone would like to take a look at it and see if it posts correctly for them.

 

It is tool #9 3/32 endmill that's causing the problem

[?Mark]

quote:

---

seems there is a G01 missing after a G03 move

---

Welcome to the club John

 

Mark

[?Mark]

Let me guess, it's a repeat pass with enter on first cut/ exit on last cut in lead in/out ?

 

Mark

[Guest]

Nope just a finish pass around the inside of a radius slot.

 

Is there any kind of work around for this Mark or is this just a situation that is/will be dealt with in MR1?

[?Mark]

Try changing plunge rate to something different than

feed rate (courtesy of Jimmy I think ?)

CNC Software is working on it (if this is the same problem )

hth

 

Mark

[Guest]

Damn,

 

Change the plunge rate and I get code that works.

 

 

How the heck does that happen?

[jplecan]

I looked at the chained geometry and the arcs weren't 180 degrees. I retrimmed the ones at 6 and 9 oclock so they were 180 deg and they posted ok. I couldn't get the other two trimmed to 180 deg. Changing plunge rate didn't help me any.

 

Jim

[?Mark]

Look here

 

Mark