[QuinnSjoblom]

I've recently started using the tool table to make use of tool length offsets. Got everything working fine. Mach3 pulls the appropriate z offset from tool table during a tool change. Only issue is, the tool info display is not showing the tool number and info. Is this not something that happens automatically? Do I need to put something in my m6 macro to make it happen? Using standard screen set and if I remember correctly, I might not be on latest mach3 version. I think there was an older version recommended for using with my Ethernet smoothstepper, I'll have to look but I seem to remember 62 being in version number, I'll check that when I get home if it's relevant

[Bob La Londe]

You have to output in code for your tool changes.

T(x) M6 G43 H(x)

Yes, I think its stupid, but that's the way it is. I considered trying to modify my tool change macro to do that, but I found it was easier to modify my CAM post processor to do it. For convenience you may want to setup your tool change macro to move to safe Z height for the tool change. If you move in X&Y for the tool change you may want to also want to save the current X&Y before the movement, and return to it at the end of the macro. Many CAM programs do not output all coordinates for the first move if the machine was at that that coordinate at the end of the last operation. Saving coordinates and returning to them prevents that from being an issue.

I would suggest when modifying a post processor you save it under a new name so you can always refer back to the original if something doesn't work the way you thought it should.

[ger21]

So if you call an T# M6 in MDI, the tool number is not changing? It should.

[Bob La Londe]

What got me is he said the offset was being applied. Only thing I thought was to show the complete required command line and hope he was just missing part of it.

[QuinnSjoblom]

no, it does not. only thing that happens in tool info window is the yellow light flashes for tool change. Number stays at 0. Although correct z offset is pulled from tool table and applied like it should. I did make some changes to my m6 start and end macro in order to send spindle to convenient location for changing the tool, could i have messed something up in the default macro that is preventing it from displaying the info? here are my m6 macros.

heres m6 start, sends my spindle to convenient xy location
x = GetUserDRO(1200)
y = GetUserDRO(1201)
z = GetUserDRO(1202)


code"G53G0 Z" & z


code"G53x"& x & "y" & y

and heres m6 end, i think i added this so i could probe for z, then press cycle start and it would automatically bring z back up to the top before moving anywhere. actually not needed anymore since i wont be probing for z between tool changes.

z = GetUserDRO(1202)


code"G53G0 Z" & z

also, heres what gcode looks like during tool change. its fusion 360 cam, standard mach3 post. the g43 comes a few lines after the tool change when the first z move happens.

(2D ADAPTIVE1)
M5
M9
T19 M6
S13000 M3
G54
M8
G0 X51.418 Y105.879
G43 Z15. H19
Z5.
Z0.25


anything look out of place?

EDIT: i just looked up what default m6 start is supposed to look like and i see:
tool = GetSelectedTool()
SetCurrentTool( tool )

is this supposed to be in my m6 start? because it isnt. is that my issue?

Edit again: Yep that was it. added those 2 lines to the beginning of my m6 and its working properly now. i must have deleted them when i first modified my m6. Thanks guys

[ger21]

Yeah, I forgot that the macro sets the tool #.

[ott12341]

if you want the tool offset to automatically go into a certain offset number in the controller , here is what you do. Activte the work offset that your using, position the X and Y axis in the normal comping position, do your comping with a 1-2-3 Block and in your program whaether the M6 program or a comp program add this line of code to it BEFORE ANY Z axis move OUT of the comp position.

G90 G10 L10 P_ R#5023;

What this does is input the current Machine position into the tool offset that you want. for instance, if I wanted tool offset number 21 to be active in the program the format would be G90 G10 L10 P21 R#5023;


P21= tool offset number we want to write to

R#5023= Current Machine Z axis position.


Hope it helped or I might be way off subjucet. lol