Improper feed rates after tool change

Hoop · Post by **Hoop** » Fri Oct 24, 2008 8:24 am

After a tool change, the speeds specified by the Gcode seem to be ignored and the rapid feed speed specified in mach 3 are used instead. Before the tool change everything works as planned.

Some decent replies on mach3 support regarding the problem:
http://www.machsupport.com/forum/index. ... 207.0.html

This is my current tool change macro:

[SEQ_PRECHAR][SEQNUM][DELIMITER]G00 Z[TOOL_CHG_PT_Z]
[SEQ_PRECHAR][SEQNUM][DELIMITER]G00 X[TOOL_CHG_PT_X] Y[TOOL_CHG_PT_Y]
[SEQ_PRECHAR][SEQNUM][DELIMITER]M6[DELIMITER]T[TOOL_NUM]
[SEQ_PRECHAR][SEQNUM][DELIMITER][SPINDLE_BLK]

This is my first load tool macro:

[SEQ_PRECHAR][SEQNUM][DELIMITER]M6[DELIMITER]T[TOOL_NUM]
[SEQ_PRECHAR][SEQNUM][DELIMITER][SPINDLE_BLK]

Do I need a G1 instruction in there so the F speed isn't ignored?

Post by **MecSoft Support** » Fri Oct 24, 2008 8:31 am

You might want to try just setting the Feedrate without a G1 in the tool change macro statement to see if the Mach3 controller will accept it.

Hoop · Post by **Hoop** » Sat Oct 25, 2008 7:13 pm

I am not sure I understand. I currently do not have a g1 in the tool change macro.

Mitch Heynick · Post by **Mitch Heynick** » Sun Oct 26, 2008 2:57 am

Well, I don't have a Mach 3, but I think the G1 is supposed to be given by the in the "Motion" section of the PP...

The variable [G_CODE] outputs the current active motion code, G0 or G1.

In my Haas tool change macro, I have a couple of more lines than you after the [SPINDLE_BLK] line:

[SEQ_PRECHAR] [SEQNUM] G54 [G_CODE] X [NEXT_NONMDL_X] Y[NEXT_NONMDL_Y]
[SEQ_PRECHAR] [SEQNUM] G43 Z[NEXT_NONMDL_Z]

Note the [G_CODE] in there. This will output a G0, however, because at this point in time, RhinoCAM tells the machine that it needs to rapid over to the G54 XY point, then rapid down to the G43 Z clearance point.

After that, the motion section should take over - that outputs the G1, because it sees a feed move from the programmed toolpath.

[G_CODE][NEXT_X][NEXT_Y][NEXT_Z]

So, check your motion section to be sure it's outputting the correct G1. If that fails, you might experiment in putting in a [G_CODE] instruction at the end of the tool change macro and see if that outputs your G1... It might still output a G0, I don't know. Otherwise, you can manually insert a G1 in the postprocessor on any line, it will output it where you insert it.

Don't know if any of this helps... --Mitch

Hoop · Post by **Hoop** » Mon Oct 27, 2008 6:26 pm

It does a little, thanks. It is clear I am missing some code from my tool change macro...

Does anyone else who uses mach 3 get g1 output after tool changes?

What is your tool change macro?

Hoop · Post by **Hoop** » Tue Oct 28, 2008 9:43 am

I'm surprised support didn't jump in with a helpful macro from the get go.

Post by **MecSoft Support** » Tue Oct 28, 2008 3:53 pm

Hoop,
Mitch had mentioned using

[G_CODE][NEXT_X][NEXT_Y][NEXT_Z]

in your tool change macros. Have you tried this?

Also you might want to specify the Feedrate as well to see if this does not affect the feedrates.

[G_CODE][NEXT_X][NEXT_Y][NEXT_Z] F [FEEDRATE]

If your G_CODE is still a G0 you might want to try

G1 [NEXT_X][NEXT_Y][NEXT_Z] F [FEEDRATE]

Hoop · Post by **Hoop** » Sat Dec 13, 2008 12:35 pm

This worked well for me.

But how can I make the tool rise to .125 during the transfer for a tool change going to 0,0,0? Not unlike "safe z" of mach3? (which doesn't seem to work during tool changes)

I would like to avoid this shaving of several thousandths upon tool change:

Do I need to set a clearance plane or does this require a macro?

Post by **MecSoft Support** » Mon Dec 15, 2008 10:30 am

You can set up the tool change point and have the tool go to this too l change point at every tool change. You will have to insert the code in the tool change macro in the post-processor to do this. If you are having trouble with this please contact us at [email protected]