M6 tool change

[Flyer295]

I'm fairly new to CNC machines so therefore easily bamboozled

Until fairly recently tool changing hasn't been an issue as I've not required it. However I've branched out into more complicated items and that's where I've hit a problem.

I have made a program, using Cut 2D and Mach 3 on the machine. It has put in a M6 code as a part of the sequence. Unfortunately the CNC doesn't obey it or if it does it's only like a hesitation.

How do I get it to raise up clear of the work and return to a (Y = 0) where I can change the tool. (All done manually)

Below is a prime example of what is not happening from a 3mm end mill to an engraving tool.

N1110G1X377.638Y12.500Z-2.000
N1120G1X377.638Y25.500Z-2.000
N1130G1X335.638Y25.500Z-2.000
N1140G1X335.638Y12.500Z-2.000
N1150G00X335.638Y12.500Z6.000
N1160T2M6
N1170 (Engraving - 20 Deg Tip 0.02 - 0.25 inches)
N1180G43H2
N1190S5000M03
(Cubby)
()
N1220G00X138.319Y118.559Z6.000
N1230G1X138.319Y118.559Z-3.000F254.0
N1240G1X138.212Y119.178Z-3.000F1016.0
N1250G1X138.121Y119.804Z-3.000
N1260G1X138.046Y120.438Z-3.000

Hope I've made it clear

Can anyone help (In layman terms please)

Bob

[cropwell]

It could be a Mach3 setting

Look in Config - General Configuration - Tool Change and see if 'Ignore Tool Change' is set on.

[m_c]

Mach 3 has various tool change settings.
It's been years since I've used Mach3, however IIRC even if it's not set to ignore toolchanges (as Cropwell has suggested), you'll still have to have suitable M6start / M6end macros so Mach3 does what you'd like it to do.

For a quick fix, you could just swap the M6 for an M00 (I can't remember if Mach3 supports M00 - Optional Stop), which will stop the machine, or split the file into separate files and run them sequentially.

[cropwell]

There are M6start and M6end macros which come as standard. If you want to move the X,Y,Z to a certain point then you will have to put that in the M6start, or just jog up and across to your tool change position. M6end will reposition the tool, but I do not remember if it switches the spindle back on.

I tend to split the Gcode into 1 file per tool.

Cheers,

Rob-T

[JAZZCNC]

Hi Bob,

Chances are that Mach is set to "Ignore tool change" like as been mentioned. Change it to "Stop Spindle wait for cycle start" not to "Auto tool changer"

Then what happens is that the motion stops at last commanded position before the M6 command then the spindle will stop. You can then Jog away to any place you like to change the tool. Then jog back and reset new Z height for new tool length. After set Z height push cycle start and the spindle will restart and motion will resume at next commanded position.

If you want to machine to move to a tool change location then the M6 start macro will need to be modified.