jog rates from gcode?

[hack613]

I'm making some tool paths where I'd like to use 10ipm for the cut rate but for this job I'd like to have the job rate also 10ipm. Catch is my mach3 is set up to jog at 180ipm.

I can just temporarily reduce the jog rate from mach3 but is there a way to have the whole job done including jogging at a prescribed rate? so I don't have to muck with mach all the time?

[hack613]

In a nutshell I'm cutting foam with a hotwire and the machine will be engaged with the material between cuts so I want to conveniently roll back the jog rate from v-carve.

Is this doable or do I have to always change my base settings in mach, then change it back after these jobs?

Thanks in advance!

[highpockets]

If I understand correctly, in the toolpath edit the tool and set the feed rate to 18 ipm.

edit: VCarve has nothing to do with the "Jog" rates in Mach3. If you want to set the Jog rate in Mach3, press the Tab key to bring up the controller.

[hack613]

Thanks!

I've been using that setting and that affects the rate of movement when cutting the material.

But when G00 (rapid) over the material it's not affected.

I can obviously go to mach and retune my motors for every job but that just seems a be excessive.

in mach there is a slider marked Rapid FRO but it seems to affect both the engaged and rapid rate...

So far the best thing I've come up with is to set the item you mentioned to 180ipm (since my machine rapids at 180ipm). then it's all the same and if I overide feed rate in mach it's all the same and I can tone it down to whatever...

Still seems a bit kludgey...

Any other thoughts?

[TReischl]

There is nothing "kludgey" about how the program is written. G0 has operated the same way from day one, which is before I started in 1974.

What you could do, is set up a post processor to output G1 instead of G0 and use that post to run the files you want to the wire to "rapid" at "feedrate". Seems simple enough to do.

Look for this in the post processor file:

+---------------------------------------------------
+ Commands output for rapid moves
+---------------------------------------------------

begin RAPID_MOVE

"[N] G00 [X] [Y]"
"[N] G00 [Z]"

Make sure you save a backup of the original post you alter and save the new one off under a different name.

[ger21]

in mach there is a slider marked Rapid FRO but it seems to affect both the engaged and rapid rate...

In General Config, Uncheck "Lock Rapid FRO to Feed FRO", and you'll be able to slow down rapids only.

[hack613]

Thanks everybody!

Those are two good solutions!

The post processor idea looks good as I can then just get rid of the rapids from my tool path.

Also the mach3/Config/General Config/Lock Rapid FRO and Feed FRO {uncheck} is a great solution too.