PDA

View Full Version : Mach 3 Tool Change Location Help?



Premiumcamper
23-10-2017, 02:40 PM
Hello Guys,

I am after a bit of guidance regarding the tool change location function within MACH 3.

I have configured my Auto Tool Zero and it is running lovely however I am unsure how to set up a certain location where it will go to before it does every tool change?

If someone would be able to help me with this it would be greatly appreciated.

Regards,

Tim

m_c
24-10-2017, 12:31 AM
You need to modify the M6start and M6end macros.

I've not used Mach 3 for a few years, so it'll probably be better searching over on the mach forums.

Neale
24-10-2017, 09:08 AM
The gcode you need is G28. This takes the machine to s predefined position, which could be your tool change position. You set the position (using machine coordinates) in one of the Mach3 configuration screens, although I can't remember which one off the top of my head. As m_c says, you can then incorporate this code into your M6start macro so that as part of the tool change operation, the machine will go to the tool change position. On my machine, I also have a fixed touch plate set into the bed at this point so I can do a "second operation" tool height setting without having to jog the tool again. When you hit "run" the M6end macro is called which by default takes the machine back to where it was when the m6 tool change started.

Premiumcamper
24-10-2017, 09:31 AM
The gcode you need is G28. This takes the machine to s predefined position, which could be your tool change position. You set the position (using machine coordinates) in one of the Mach3 configuration screens, although I can't remember which one off the top of my head. As m_c says, you can then incorporate this code into your M6start macro so that as part of the tool change operation, the machine will go to the tool change position. On my machine, I also have a fixed touch plate set into the bed at this point so I can do a "second operation" tool height setting without having to jog the tool again. When you hit "run" the M6end macro is called which by default takes the machine back to where it was when the m6 tool change started.

I thought it was as easy as adding some more vbscript into my Auto Tool Zero script already? Would this work OR does it have to be done within the M6START & END Macro?

Tim

Neale
24-10-2017, 09:48 AM
Can you explain exactly what you are trying to do? Everyone has their own way of working and I'm not quite sure what you're looking for.

For example, my tool change code moves the tool to tool change position, waits until I hit Run, then goes back to where it started and carries on. While the tool is at the tool change position, I can choose to use one of the tool-height setting options I have written or not - they are not built-in to the tool-change macros themselves. That suits the way I work, but might not be right for everyone.

Premiumcamper
24-10-2017, 10:01 AM
Neale,

When I'm running our GCODE to produce one of our units it had four cuts in total. I would like it to go to a certain position WHEN a tool change it needed then I press auto tool zero it hits my wireless probe (Which will be in a fixed location) zero's its self out and then returns to the next cutting position.

Hope this makes sense to you! :D

Tim

m_c
24-10-2017, 11:01 AM
Anything to do with toolchanges happens, or at least starts and ends in the M6 macros.

I'm not entirely sure, but I think once you've used M6start to move to your toolchange position, you can then use your tool zero button, then once you're finished and click cycle start again, M6end takes care of moving back to the work area.

Neale
24-10-2017, 11:05 AM
Anything to do with toolchanges happens, or at least starts and ends in the M6 macros.

I'm not entirely sure, but I think once you've used M6start to move to your toolchange position, you can then use your tool zero button, then once you're finished and click cycle start again, M6end takes care of moving back to the work area.

Exactly. This is what I do on my own machine. All you need to do is put a move (in machine coordinates) to the touch plate location into the tool height set macro and the job's a good'un

Premiumcamper
24-10-2017, 12:48 PM
Neale could you copy and paste what's inside your M06.M1S file please?

Regards,

Tim

Neale
24-10-2017, 12:54 PM
Can do - will take a little time as I'll get the current copy off my machine. Might as well post m6start, m6end, and my tool-height setting routine while I'm at it. These all work, at least on my setup.

Premiumcamper
24-10-2017, 12:55 PM
I have the auto tool zero function working.

Just struggling to set up the location, but that would all be fantastic.

Thankyou.

Neale
24-10-2017, 01:47 PM
So, this doesn't do exactly what you need, but it might help a bit.

23098

I suspect that what you need is something like:

code "g53 g0 x[your tool change X] y[your tool change Y]"

somewhere near the top of your tool height set macro. Note the G53 - this is important as it means "use coordinates on this line as machine, not work, coordinates"

Can you post your tool height set macro?

Premiumcamper
24-10-2017, 01:59 PM
So, this doesn't do exactly what you need, but it might help a bit.

23098

I suspect that what you need is something like:

code "g53 g0 x[your tool change X] y[your tool change Y]"

somewhere near the top of your tool height set macro. Note the G53 - this is important as it means "use coordinates on this line as machine, not work, coordinates"

Can you post your tool height set macro?

Hello Neale, I have sent you a email directly to you.

Regards,

Tim

Premiumcamper
25-10-2017, 12:32 PM
So, this doesn't do exactly what you need, but it might help a bit.

23098

I suspect that what you need is something like:

code "g53 g0 x[your tool change X] y[your tool change Y]"

somewhere near the top of your tool height set macro. Note the G53 - this is important as it means "use coordinates on this line as machine, not work, coordinates"

Can you post your tool height set macro?

AUTO TOOL ZERO SCRIPT:-


FeedCurrent = GetOemDRO(818) 'Get the current settings, OEM DROs (818)=Feedrate DRO
ZCurrent = GetOemDro(802) 'OEM DROs (802)=Z DRO
GageH = GetOEMDRO(1001) 'OEMDRO(1001)=Gage Block Height
ZNew = ZCurrent - 300 'probe down 20 mm

Code "G90F500" 'slow feed rate to 100 MM/MIN
Rem Code "G4 P1" 'Pause 1 second to give time to position probe plate
Code "G31 Z" &ZNew
While IsMoving()
Sleep(10)
Wend
Call SetDro (2,GageH) 'DRO(2)=Z DRO

FinalMove = GageH + 10
Code "G0 Z" &FinalMove
Code "F" &FeedCurrent 'restore starting feed rate dr.lin 2009.10.16

Premiumcamper
27-10-2017, 11:56 AM
This thread can be closed now.

All resolved thanks to Mr Neale.

Thank you again for all your guidance.

Tim

Premiumcamper
27-10-2017, 11:56 AM
This thread can be closed now.

All resolved thanks to Mr Neale.

Thank you again for all your guidance.

Tim