Build Thread Mach3 to Acorn

[Leo Voisine]

Trying to get tool touch off to work.

TT4

My machine does not have ATC. Only one tool at a time in an ER20 collet

I do run jobs that use as many as 4-5 cutters.

I want to be able to use the TT4 to set my tools.

I have tried several times making different settings in the wizard but I am not getting what I want. Maybe what I want is not possible.

I have not used tool height on my home router with Mach3. That was done by setting the part zero with a tool, then at every tool change resetting Z for the new cutter on the part zero surface.

I would like to have TT4 in a fixed location on the machine. I am thinking X1.0 Y1.0 from machine home on a steel plate that is about 1/4 thick. At each tool change I want to be able to move the the TT4 set the new tool and continue the program on the workpiece.

Am I asking for something that cannot be done?

[Sword]

Yes, it can be done. Your M6 (mfunc6.mac) macro will need to be set up for it, or you can use Swissi's CHIPS add-on to do that and more.

Related reading...
https://centroidcncforum.com/viewtopic.php?f=63&t=1493

I use CHIPS now, but for quite a while, I used the attached macro. I haven't updated this macro to work with the latest version, but it shouldn't take too much editing to make it right. It presents you with three choices when a tool change is called (M6). Set with moveable plate and save offset (goes to a fixed touch off to get/save offset after using a touch plate), use current offset with fixed TT, or movable plate only. Could probably add another choice to continue without resetting (using the same tool again).

Your Return Points for the fixed tool touch off also need to be set in CNC12 (my file uses G30P2). A manual tool change location could also be set with G28 or one of the other G30P's.

[Leo Voisine]

Ahhhh OK. So what I want is achievable, but. I love learning new stuff and this is going to be fun. I did look at the link to another thread and I liked the video from ?scott? That is better than what I was thinking about. I like the bit about learning and diving into the macros. This is gonna be sweet. I am going to study this a bit more.

[RogDC]

Leo,
You can enter the machine coordinates for your fixed TT in g30 P3. This can also be configured on the TT page in the Wizard which writes the fixed TT location to G30 P3.

I have ATC so I'm a bit out of practice on the manual tool changes.

CHIPS can be configured to measure the tool offset after each tool change.

[ShawnM]

Yes Leo, this can be very easily accomplished. There’s a whole topic here on the forum with macro examples for exactly what you wanna do. I worked with non-ATC machines for a couple of years and having an M6 macro that auto measured tools between tool changes was a game changer.

[Leo Voisine]

I am thinking that T1 should be set on TT4 tool touch probe then used to set part zero.

After part zero is set then each tool should be numbered T2, T3 and so on and those are the tool changes to be set on TT4 tool change as reference tools?

In the wizard then Z-zero = reference ?

In Vectric all tools are T1, but I think I can change that accordingly

I have not tried any of that yet.

[Leo Voisine]

I just made a 3D bas relief program in Vectric using three tools

I could change tool numbers ------ with Mach3 I never changed the tool number. Centroid is more like the industrial machines. I do understand that strategy.

So in Vectric I used T1, T2 & T3
I posted with Centroid all the tools into one file
Looking at the Gcode I see the T1 M6 and the H1

Now I get the Mfunc6.mac function
That is where the Tool touch come in
M6 will allow me to change the tool - measure the tool then continue the program until the next M6 is executed.

I do see the fixed position in the wizard.

Am I getting close?

[Leo Voisine]

I am getting into the Centroid part of operating my new machine. This is not my old Chinese Mach3 machine for sure.

So this is configuring my new machine to my liking

I would prefer to have each of my 3 axis's move off the limit switches than they do now.

Looking at the cncm.mac file I see

;Perform Homing commands
M92/Z L1
M26/Z
M91/Y L1
M26/Y
M91/X L1
M26/X
M26/A

If I add a .125 move as shown below, will that cause a problem?
Is there a better way to do this?

;Perform Homing commands
M92/Z L1
Z-.125
M26/Z
M91/Y L1
Y.125
M26/Y
M91/X L1
X.125
M26/X
M26/A

[Gary Campbell]

Leo...
That won't work as the axes are not necessarily at the zero position prior to being set at machine zero by the M26 command.

After the M91/92 command, use a relative (G91) move

M92/Z L1

M91/Y L1

M91/X L1

G91 X0.125 Y0.125 Z-0.125
G90

M26/X
M26/Y
M26/Z
M26/A

[Sword]

Yep with what Gary said. Here's another example that I run on my machine.

Code: Select all

M92/Z L1         ; Move + to Z prox
M26/Z

M91/X L1         ; Move - to X prox
G91 G0 X3.3988   ; Move X required distance from prox to table X home

M91/Y L1         ; Move - to Y prox
G91 G0 Y1.9231   ; Move Y required distance from prox to table Y home

M26/X/Y          ; Set Machine home at current location
G90              ; Return to absolute positioning
M225 #105 "** Machine home set, have a G90 great day! **"