How to disable the I and J output in Fusion 360 3d program CAM

[Aadithya01]

Hey can anyone tell me how to disable the I and J coordinates in the output cam Program for FANUC 

[LibertyMachine · Accepted solution]

For XYZ motion or 4th axis movement?

If the former, there is a toggle at the Post Process screen; useRadius

Setting it to "Yes" will output "R's" instead of I and J

[George-Roberts · Accepted solution]

Or if you want to get rid of arcs altogether, in the post processor, change allowedCircularPlanes from undefined to 0. This will linearize all arcs

[Aadithya01]

HEy @George-Roberts

For the fanuc post processor i dont have the option for allowedCircularPlanes ... 

[Aadithya01]

Hey @LibertyMachine @George-Roberts

Do you know how to disable T01 M06 line from the post program output for fanuc .. My customer had asked this .. cause his CNC machine doesn't have a tool magazine .. so is there any setting in Fusion 360 to disable the T01 M06 line. 

[LibertyMachine · Accepted solution]

I would look at the posts for the Mach3 or the Tormach. Both of those have toggles for "changeTools" or something to the effect

Of course, you could also brute force it and delete the section in RED

    disableLengthCompensation();
    writeBlock("T" + toolFormat.format(tool.number), mFormat.format(6));
    if (tool.comment) {
      writeComment(tool.comment);

[ivan.stanojevic · Accepted solution]

---

@Aadithya01 wrote:

HEy @George-Roberts

For the fanuc post processor i dont have the option for allowedCircularPlanes ... 

---

Yes you have at the beginning of every post.

[Aadithya01]

I just did this 

// writeBlock("T" + toolFormat.format(tool.number), mFormat.format(6));

I just added the // backslahes and that worked . Many thanks @LibertyMachine

[Aadithya01]

Hey @LibertyMachine @ivan.stanojevic@George-Roberts

T1 M06 is sucessfully diabled 

How to disable H01 ... ??

[ivan.stanojevic]

Search for:

hFormat.format(lengthOffset)

and delete it.

[Aadithya01 · Accepted solution]

Error(C:\POST PROCESSORS\fanuc.cps:1049): ReferenceError: f is not defined

After deleting H offset  like you said it is saying the above error 

Please see the attached fanuc post processor where I had made the change

[ivan.stanojevic · Accepted solution]

You have a typo.
Delete letter f on the 1049 line.