Change tool & tool length compensation

[nio]

Hi,
after some days fighting with mach3, i need help with this if it's possible...
Firs of all, thank you for any tips you could give me...
- Is it absolutely necessary limit switches for a change tool procedure?? now i havent' got installed, now i'm working with soft limits.
- Now i know how i have to do to change tool when the mill is exactly the same length, but my problem is when the tool is different length.... i was looking information in mach3, and i finished in a offset you have to mark in each tool you have in mach3,so

Anybody has done this procedure???? Could you explain me the process??

Probably i need a probe to the Z axis, isn't it??

Thanks in advance...

[Improbable Construct]

I do not have any limit switches installed in my setup, so no you do not have to have them.
I don't even have soft limits set.
I let the CAM software take care of the tool offsets.
As far as Mach3 is concerned every tool is tool #1.
I break my G-code up into sections based on the tool.
It is not unusual for me to have 5-10 G-code files for one part.

A touch probe for the Z-axis is the easiest way to reset after a tool change.
It is a pain to set up but once its done you don't have to change it again.
If you want I can send you the screen set I use. It should have touch probing set up for mm units.

[nio]

Hi IC,
so if i understand right, you break you G-CODE file, you mean, you have separate files and you load each once a time in the mach3??? so if yes, how you homing X,Y when you load a new file??? with a mark?? o how?? because you should start in the same position you started the first time, no??

When you refere to a screen set you mean BlueScreen plugin for mach 3, isn't it?? that's i've got installed....

Thanks again!!!!

[Improbable Construct]

Right, I break up my G-code.
So I might have a file that pockets an area with a 1/4" endmill.
Then I might have to change to a 1/8" endmill and finish the pocket.
Then I may have another file that cuts some holes.
Then another one that cuts the outside profile.

Before I start I decide where 0,0 will be. Maybe it is the center maybe it is a corner.
Once you tell Mach3 where that is and zero out x and y, Mach3 will remember where that point is as long as you do not unlock your motors.
If you hit reset or your E stop then it all falls apart...
You can load new G-code and Mach3 will start from the same point.
From there you can swap tooling and all you have to do is reset your Z zero.

I do use the MachBlue with probing screen set.

[nio]

OK IC, i'll try to do it in that way....

Thanks again

[sectorix]

Someone should really do a video on a tool change with a grblShield
cant find anything that I can relate to

[crazeegeek]

Someone should really do a video on a tool change with a grblShield
cant find anything that I can relate to

This video covers a basic (manual) method to this, using a stock shapeoko2(grbl and dremel), makercam, and ugs. Of course having homing switches installed would make things even easier.

https://www.youtube.com/watch?v=qf-EAbFD11s

[Estlcam]

Hi,

you don't need to split up your G-Code - just insert a tool change command.
There are several ways to do this - but for manual changes this will do:

Code: Select all

M05
M00
M03

• M05 stops the spindle (if it is controlled by Mach3)
• M00 stops the machine so you can change the tool
• M03 restarts the spindle

Usually your CAM program should do this for you automatically if you use more than one tool.

The tool change itself with tool length compensation works this way:

• After M00 stopped the machine you can move it manually to any position you like so you can release the old tool...
  Don't worry about changing the position - the machine will later automatically return to the right position...
• Insert the new tool...
• Finally touch the Z-Axis off with the new tool against the same surface you used to touch off the old tool -> tool length is now compensated.
• Continue the program...

You don't need limit switches for manual tool changes. They are only necessary if you have an automatic tool changer / automated tool length sensor or if you expect the machine to return to a dedicated "home" position for changing.

Christian

[Okinawanwinds]

• M05 stops the spindle (if it is controlled by Mach3)
• M00 stops the machine so you can change the tool
• M03 restarts the spindle

Usually your CAM program should do this for you automatically if you use more than one tool.

The tool change itself with tool length compensation works this way:

• After M00 stopped the machine you can move it manually to any position you like so you can release the old tool...
  Don't worry about changing the position - the machine will later automatically return to the right position...
• Insert the new tool...
• Finally touch the Z-Axis off with the new tool against the same surface you used to touch off the old tool -> tool length is now compensated.
• Continue the program...

You don't need limit switches for manual tool changes. They are only necessary if you have an automatic tool changer / automated tool length sensor or if you expect the machine to return to a dedicated "home" position for changing.

Christian

Hello Christian,

I am a newbie Estlcam user and I would ask a question.
For M00 and M06(tool change), what is the difference of them actions?
I thought M06 is the manually bit-change command.

Thank you, Okinawanwinds

[johnbeck7799]

Hi,
after some days fighting with mach3, i need help with this if it's possible...
Firs of all, thank you for any tips you could give me...
- Is it absolutely necessary limit switches for a change tool procedure?? now i havent' got installed, now i'm working with soft limits.
- Now i know how i have to do to change tool futuristic clothing when the mill is exactly the same length, but my problem is when the tool is different length.... i was looking information in mach3, and i finished in a offset you have to mark in each tool you have in mach3,so

Anybody has done this procedure???? Could you explain me the process??

Probably i need a probe to the Z axis, isn't it??

Thanks in advance...

I do not have any limit switches installed in my setup, so no you do not have to have them.
I don't even have soft limits set.