CAM Expert - increase precision or use radius

[rincewind23]

Hi all,

I've built a CNC mill and I'm just looking at software now. I am using EMC2 on Linux to run the mill, and I'm evaluating CAM Expert for generating the GCode after drawing a test plan in QCad demo.

Unfortunately EMC barfs on my GCode - I get the "radius to end of arc differs from radius to start" error. After some research it appears to be due to rounding errors when using I and J with a G02/G03 code. This seems to be confirmed as the error tells me r1=3.0000 r2=3.0008 for a 3mm radius arc.

Is there a way to turn up the precision in CAM Expert, or use R instead of I and J in the GCode? I added a decimal place to the precision in drawing preferences, but it generated the same gcode.

Cheers,
KEv.

[andrew]

All configuration for CAM output is done in the machine configuration file you can find in the directory "machines" of your CAM Expert installation.

For example machines/gcode.cxm.

You can edit the file with a plain text editor of your choice.

To increase precision:

Code: Select all

[Standards]
Digits = 4


Or any number that indicates the number of digits after the dot.

To switch from using I/J to R, you have to adjust the OrderArcCW and OrderArcCCW as follows:

Code: Select all

OrderArcCW
  {<NewLine>N<Number> G02 X<X2Abs> Y<Y2Abs> R<Radius>}

OrderArcCCW
  {<NewLine>N<Number> G03 X<X2Abs> Y<Y2Abs> R<Radius>}


Or similar. For a reference of available configuration options and commands, please refer to the manual at:
http://www.ribbonsoft.com/camexpert/man ... ter05.html

[rincewind23]

Thanks for the reply. I did read that documentation page but I must have been reading too fast as I missed the [standards]digits setting.

I did see the sections on OrderArcCW and OrderArcCCW for changing I/J to R, but when I changed those in my machine, the GCode generated no longer contained any curves.

I tried the code for these in the format in the documentation and the format you specified in your reply (your reply doesn't have <delmod:1> after the G02), but with the same result both times.

Is this to do with the fact that the demo camexpert is only version 2.0.4.8 while the release version is 2.4.6?

I changed the digits to 5 and now the EMC simulator is running fine once I remove the first generated line (G00 Z100.000). It seems strange to try and set the Z axis to 100?

Thanks for the help. And if you could confirm that 2.0.4.8 is the latest demo version, that would be great too.

[andrew]

when I changed those in my machine, the GCode generated no longer contained any curves.

Please check the generated code against the documentation for your specific machine. G-code is an extremely flexible 'standard' and every machine controller has its own set of commands.

Is this to do with the fact that the demo camexpert is only version 2.0.4.8 while the release version is 2.4.6?

No. You really need to go over the generated G-code manually during the configuration phase.

I changed the digits to 5 and now the EMC simulator is running fine once I remove the first generated line (G00 Z100.000). It seems strange to try and set the Z axis to 100?

Here also, every machine operates differently. You definitely will have to adjust this to fit your specific needs. gcode.cxm is provided as an example configuration only.

Thanks for the help. And if you could confirm that 2.0.4.8 is the latest demo version, that would be great too.

Yes, 2.0.4.8 is the latest.