Camsoft Lite G02/G03 Error

[DBM1]

I get an error every time I try to run a G02 or G03 code.

With the parameters set to absolute when I run.

G90 T1M6
G05
G17
G01 Z-.1 F75.
G02 X1. Y1. I1.
G01 Y2.
G02 X2. Y3. I2. J2
G01 Y4.
G01 X1.
G03 X0. Y3. I1 J3
G01 Y0.
M30

I get the error "Start Radius of Arc Differs from end Radius"



With the parameter set to incremental and I run the code:

G91 T1M6
G06
G17
G01 Z-.1 F75.
G02 X1. Y1. I1.
G01 Y1.
G02 X1. Y1. I1.
G01 Y1.
G01 X-1.
G03 X-1. Y-1. J-1
G01 Y-3.
M30
%
M 30

I get the same error.

If I set the parameters to Radius and run the code:

G90 T1M6
G17
G01 Z-.1 F75.
G02 X1. Y1. R1.
G01 Y2.
G02 X2. Y3. R1.
G01 Y4.
G01 X1.
G03 X0. Y3. R1.
G01 Y0.
M30

I get the error "Radius is zero, Illegal Command"

When I run these through my tool path plotter program they run fine. I am lost here, and suggestions would be appreciated. It is hard to have a milling program without a G02 or G03 anywhere for the type work we do.

Please let me know if any more information would be helpful.

Dan

[camsoft]

Dan,

All 3 versions of the G code run through without error producing the same shape as long as you have the FANUCARC check box set correctly before loading each G code file version on the TOOL PARAMETER screen or else on the SETUP screen under General Settings.



Tech Support
CamSoft Corp.
support@camsoftcorp.com
PH 951-674-8100
Fax 951-674-3110
www.cnccontrols.com

[DBM1]

Card is set to GALIL. All other G Code programs run without error as long as there is no G02 or G03.

Dan

[camsoft]

We have ours set to Galil mode as well.

All 3 run through fine, no errors in Galil mode.

It's not the Galil mode setting that matters. It's the FANUCARC setting for Absolute, Incremental or R code for radius choice that makes the difference when using G2's or G3's.

Also if you have CNC Pro there's the R value in the G code file. It you use CNC Lite or Plus or either CNC Pro in Absolute or Incremental mode the R value won't matter.


Tech Support
CamSoft Corp.
support@camsoftcorp.com
PH 951-674-8100
Fax 951-674-3110
www.cnccontrols.com

[DBM1]

Perhaps I should go over the steps I take again:

Step 1 Boot PC
Step 2 Start CamsoftLite
Step 3 Click on the little tool box and set FANUC ARC Centers to absolute (0), click the little check mark to close screen.
Step 4 Load absolute program
Step 5 open MDI screen to see current program
Step 6 Verify I have opened the absolute program
Step 7 close MDI window
Step 8 click Cycle Start
Step 9 Get Error message

I then exit the program and start new, this time Step 3 is set arc centers to incremental Step 5 load incremental program

Same routine for Radius

I have spent hours trying everything I can think of and am still getting errors.

Thanks again

Dan

[camsoft]

Dan,

That's good. We used the same steps and it works okay.

Are you sure you have the Machine type set to MILL3D? And not Lathe or some other machine type?

If not under General Setting enter MILL3D in the MACHINE TYPE box.

If so using SETUP , RESTORE the CNCLITE.CBK file and run your "Incremental G code" program through.

If it works then you'll need to contact us to give us your latest CBK file so we can investigate the settings in your CBK.

If CNCLITE.CBK doesn't work then we need to talk to you on the phone "live" to figure this out, get your company name , serial number and version ect...

[DBM1]

I am sure we are set to Mill3d.

I will try your suggestion tomorrow with the CBK file and get back to you.

thank you

Dan

[Karl_T]

Originally Posted by DBM1 I get an error every time I try to run a G02 or G03 code. With the parameters set to absolute when I run. G90 T1M6 G05 G17 G01 Z-.1 F75. G02 X1. Y1. I1. G01 Y2. G02 X2. Y3. I2. J2 G01 Y4. G01 X1. G03 X0. Y3. I1 J3 G01 Y0. M30 I get the error "Start Radius of Arc Differs from end Radius" ... Dan

I only looked at the first part of this one. I can see it won't work, you got to command the machine to the correct start position with a G0 or G1 before the first G2. (The x and y values could be anything)

Try this, set FANUCARC=0 then run this

G01 X1 Y0 F10
G02 X1 Y0 I0 J0

Your should get a full circle.

Karl

[DBM1]

Thanks,

I first park the mill at z-12 y-7 z0 before I cycle start. This put the table in the center of the travel. Will try your code tomorrow.

Dan

[DBM1]

Originally Posted by Karl_T I only looked at the first part of this one. I can see it won't work, you got to command the machine to the correct start position with a G0 or G1 before the first G2. (The x and y values could be anything) Try this, set FANUCARC=0 then run this G01 X1 Y0 F10 G02 X1 Y0 I0 J0 Your should get a full circle. Karl

I tried this today and it worked great. At least now I know the mill can do a circle. Karl, could you put together a few lines of code for a G02 X Y R test (FANUCARC=R) so I can check that one.

Thanks again

Dan

[Karl_T]

Originally Posted by DBM1 I tried this today and it worked great. At least now I know the mill can do a circle. Karl, could you put together a few lines of code for a G02 X Y R test (FANUCARC=R) so I can check that one. Thanks again Dan

set FANUCARC=2.

Modify your G02 and G03:

QUESTION 131
How do I use the R Code for turning a radius instead of I, J & K?

The first thing to do is to use the CNCSETUP.EXE program to set the FANUCARC parameter to equal 2. The second thing is change the format of the CW and CCW commands in your GCODE.FIL file for G02 and G03 to the following format:

EXAMPLE: CW x;y;z;r
CCW x;y;z;r

(I don't have time tonight, but I could write you a G02 and G03 that does both i,j and r. Tell me what custom G code numbers your'd like to call to do the switch. kinda like G90 is abs and G91 is inc.)



Run this gcode

G01 X1 Y0 F10
G03 X0 Y1 R1

You'll get 90 degrees CCW starting at 1,0 and ending at 0,1

[Karl_T]

Here's some untested code to switch among the three FANUCARC modes. I'll use G95 to set absolute arc centers, G96 for incrmental arc centers, G97 for radius arc designation.

In startup.fil, define your default. Add these lines

FANUCARC=0 'absolute arc centers
\75=0 'arc type, 0 is abs.

modify your gcode file


FANUCARC=0
\75=0
MESSAGE Absolute arcs
--G95
FANUCARC=1
\75=1
MESSAGE Incremental arcs
--G96
FANUCARC=2
\75=2
MESSAGE radius arcs
--G97


here's my existing G02, yours may be different

DISPLAY4 {f}
DISPLAY5 {s}
TIME CYCLE;\4
DISPLAY7 \4
RUNTIME \4
DISPLAY8 \4
CW x;y;z;i;j;k
-----G2

Let's make it like this:

DISPLAY4 {f}
DISPLAY5 {s}
TIME CYCLE;\4
DISPLAY7 \4
RUNTIME \4
DISPLAY8 \4
IF \75<2 THEN CW x;y;z;i;j;k
IF \75=2 THEN CW x;y;z;r
-----G2


Do the same for G3


NOTE: i write for Pro, your version has a ! in front of every line. And less commands, I don't know which ones you're missing.

Now just write the arc type in your Gcode:

G1 X1 Y0 F10
G95
G2 X1 Y0 I0 J0 'full circle
G96
G2 X1 Y0 I-1 J0 'ANOTHER FULL CIRCLE IN INCREMENTAL
G97
G2 X0 Y1 R1 '90 DEGREE ARC


karl

PS I probably left at least one error for you to find.