M6 Macro and G43

[corbin]

Hi everyone!
I've got an Avid CNC with Centroid/Acorn. I've been discussing with Eric at Avid about the M6 macro, in particular how their M6 macro also calls G43 to activate the tool height. I thought this was really strange, as M6 is just a tool change, and the calling GCode should later do a G43 to activate the tool's height offset.

Should an M6 macro also call G43?

Why/Why not?

Isn't it the post processor's job to do an M6 followed by a G43?

Thank you,
Corbin

[cncsnw]

There is generally no harm to having a G43 in an M6 macro, but you are right that it is generally the responsibility of the G code program (and thus the programmer or postprocessor) to put in a G43 after the M6.

If including the G43 in the M6 macro encourages people to omit it from the CNC programs, then that is just asking for trouble later. The resulting CNC programs are no longer portable from one machine to another, and a support tech who looks at the CNC program is going to flag the lack of G43 as a likely cause of Z height problems.

[corbin]

If including the G43 in the M6 macro encourages people to omit it from the CNC programs, then that is just asking for trouble later. The resulting CNC programs are no longer portable from one machine to another, and a support tech who looks at the CNC program is going to flag the lack of G43 as a likely cause of Z height problems.

I agree, it is innocuous to have the M6 do a G43; I can't think of a case where it wouldn't need to match up with the tool.

I think this is the biggest problem with Avid's implementation: they emit the G43 call from their Post Processor and assume the M6 does it, but a lot of DIY' people's M6 doesn't do it, because...well, it doesn't have to!

Maybe I should just go ahead and add it to my M6, unless anyone can think of a reason not to.

Corbin

[Gary Campbell]

Agree wholeheartedly with Marc, but would like to add that a large number of non professional users have a propensity to do manual tool changes when using ATC equipped machines.

They seem to always get the tool changed, but seldom remember to toggle on the tool offset, and then of course, set their part zero with no tool offset applied. The issue is compounded during a cut file when there is a tool change mid file, and cutting resumes with an out of whack part zero.

I fought this for a long time as I have nearly 50 ATC customers that came to Centroid and ATC from collet spindles on hobby controllers like Mach or ShopBot. In many cases, after months or longer taking support calls from about 10% of these users I have bit the bullet and added the G43 line to the M6.

So, knowing where Corbin is coming from, I am sure that it will be added as that is the path of least resistance when compared to properly training operators. I also have seen no negative results from a double or redundant G43 call in both the M6 and postP.

With that said, I am a bit embarrassed by how much the consumer CNC router world (and my part in it) has dumbed down CNC operation over the last 20 years. Hopefully Centroid will stick to their tried and true and keep a version that requires a trained operator. Not everything has to be idiot proof.

[cncsnw]

Nothing wrong with making it idiot-proof, as long as you don't actively undercut the trained operator.

Supporting the operator who calls up a tool with M6, then proceeds to use it manually (or use it for part setup without going through the Part Setup screen) is a good reason to include the G43 H__ code in an M6.

[corbin]

Thanks everyone! I think I'm convinced that I should add the G43 to my M6.