[RedStar2016]

Here is a little back ground info.
I have replaced the computer that operates our plasma table as the fan cooked and we had another xp computer.
I loaded mach 3 and copied our licence over and everything works well except now the whenever I have a round part that has a protrusion or fillets the mach 3 doesn't know what to do and the part does not carry over. Im not good at the programming part of things and think it must be an easy fix but I cant seem to resolve. I changed the IJ to incremental and absolute and no luck. If someone has dealt with this or know of a fix I would greatly appreciate your input. Pictures are attached.

I would also like bobcad to not generate the following lines of code as i manually have to delete them otherwise my plasma will cut across the sheet when i completes a part. If someone knows about that too. Its not a big deal.
N19 G53 Z0
N20 G53 Y0

This is my G Code in Bobcad

Im hoping all my pictures work out.

[mactec54]

RedStar

The IJ have to be set as incremental, the distance is Absolute, which you have, even if it does not solve the problem, this is the normal why to use those 2 settings, you are not using I & J's in your program, you have Radius

There may be something under ToolPath Config, but I don't know of any setting for using Radius

The G53 at the beginning of the program needs to be gone also

If you do a G0 Z0. then a G53 Y0. this most likely will work better

Check in Bob Cad if you have a setting to use I & J's and then try that program

[BurrMan]

Here is a little back ground info.
I have replaced the computer that operates our plasma table as the fan cooked and we had another xp computer.
I loaded mach 3 and copied our licence over and everything works well except now the whenever I have a round part that has a protrusion or fillets the mach 3 doesn't know what to do and the part does not carry over. Im not good at the programming part of things and think it must be an easy fix but I cant seem to resolve. I changed the IJ to incremental and absolute and no luck. If someone has dealt with this or know of a fix I would greatly appreciate your input. Pictures are attached.

I would also like bobcad to not generate the following lines of code as i manually have to delete them otherwise my plasma will cut across the sheet when i completes a part. If someone knows about that too. Its not a big deal.
N19 G53 Z0
N20 G53 Y0

So 2 things. First, the g53 thing is in the post processor of bobcad. Easy enough to change, but:

Second, so nothing had changed with "BOBCAD" do to the fry? Or what?

Are you running gcode that "used to work fine" or are you generating new stuff from a new install of bobcad.

The g53 could work. Its a machine home and needs to have machine and workoffsets setup in mach properly...

If it is "ONLY" a mach change, there are a couple more files to copy over, OTHER than the license file, that will get your mach back to where it was....

[The Engine Guy]

To have BobCAD outputting I and J for arcs instead of R then open your Post Processor in Notepad and go to line :-

222. Arc center a=absolute, b=incremental, d=unsigned inc., e=radius? b

If it is as above then it will output I and J for the arcs, if it has an e there at the end of the line instead of a b then it will output an R for arcs, modify as required

To remove the G53 at the start of the program go to Line :-

2. Start of file Standard
n,"(PROGRAM NAME - ",prog_name,")"
n,measure_mode
n,"G53",absolute_coord,"G40"
n,lpw_power_setting,"(POWER SETTING)"
n,rapid_move,lpw_torch_height_control
n,rapid_move,force_x,xr,force_y,yr

To stop the G53 move being generated simply delete the "G53", in Blue shown above and Save the PP, don`t do a "Save as" because it will be saved as a .txt file and will no longer be a Pst file, just do "Save".



As for removing the G53 moves at the end of the program go to Line :-

5. End of file for non-zero tool
n,"G53 Z0."
n,"G53 Y0."
n,"M02"
"%"
To stop the G53 moves being generated simply delete the two lines in Blue shown above and Save the PP, don`t do a "Save as" because it will be saved as a .txt file and will no longer be a Pst file, just do "Save".

Hope that`s of some help to you.

Usual disclaimers apply, use at own risk

Regards
Rob