topic Re: No G28 in the beginning in Fusion Manufacture Forum

No G28 in the beginning

Anonymous — Sat, 14 Oct 2017 20:59:53 GMT

Does anyone know how to modify a generic post processor, like Fanuc to disable G28 in the beginning of a program? Our company doesn't need it.

N10 G90 G94 G17 G49 G40 G80

N20 G28 G91 Z0.

N30 G90

How to remove N20 and N30 blocks?

Thanks

Re: No G28 in the beginning

daniel_lyall — Sun, 15 Oct 2017 06:38:25 GMT

Set show sequence numbers to no for N10, N20 so on that will stop N, why G28, it can be removed with a post processor edit

Re: No G28 in the beginning

GeorgeRoberts — Sun, 15 Oct 2017 14:29:14 GMT

Hello,

Thanks for posting. The G28 safe retract line is put in the post processors to ensure the machine is at a safe Z position prior to any movements that could cause issues. If you would like to remove the G28, please ensure you enter in a sensible safe retract line to replace it.

Cheers

Re: No G28 in the beginning

Anonymous — Sun, 15 Oct 2017 16:34:13 GMT

I figured it out: moving the } to new place. Thank all of you!

// stop spindle before retract during tool change
if (insertToolCall && !isFirstSection()) {
onCommand(COMMAND_STOP_SPINDLE);
// } (removed } )

// retract to safe plane
retracted = true;
writeBlock(gFormat.format(28), gAbsIncModal.format(91), "Z" + xyzFormat.format(0)); // retract
writeBlock(gAbsIncModal.format(90));

} //added } here

Re: No G28 in the beginning

GeorgeRoberts — Mon, 16 Oct 2017 07:24:14 GMT

Hello,

Thanks for posting your progress. Moving the bracket there will still output G28 on toolchanges (if it is not the first one). You can comment out the single line by using two forward slashes '//'. To actually remove this line, change it from this:

 writeBlock(gFormat.format(28), gAbsIncModal.format(91), "Z" + xyzFormat.format(0)); // retract

to this:

// writeBlock(gFormat.format(28), gAbsIncModal.format(91), "Z" + xyzFormat.format(0)); // retract

Re: No G28 in the beginning

schlotterbeckmachine — Tue, 04 Jun 2019 21:15:50 GMT

This solution removed G28 from the beginning only, correct?

Re: No G28 in the beginning

daniel_lyall — Tue, 04 Jun 2019 21:22:19 GMT

Depending on what is in the post now a lot of posts are different now compared to 2 years ago.

Re: No G28 in the beginning

schlotterbeckmachine — Tue, 04 Jun 2019 21:25:29 GMT

In this particular case it is generic fanuc turning that's had some edits made. I'd like to keep G28 prior to tool changes but want it cut out at program start.