Manual Tool Change with ATC Spindle

[metzenovich]

I have a Colombo RC110 ATC spindle on my CNC retrofit. I've been able to get the individual air relays hooked up to the TTL outputs and I've been able to do a very manual tool change by individually turning the TTL outputs on and off in the right order / timing.

What is the correct way to do a manual tool change with an ATC spindle? The CNC I inherited no longer has the ATC carousel and it will be a while before I can make one.

Is there a built-in Masso way? Or should I just write G-code that does it with M00, M10, M11, etc?

 

[testyourdesign]

@metzenovich

Considering that you don't have the ATC carousel, you probably shouldn't use the ATC functions just yet. I would set the Masso controller to use Manual Tool Change for now.

I connected my drawbar control to a momentary switch on the mill head so I can actuate the drawbar manually. By setting the controller into manual tool change mode a T# M6 command will automatically stop the spindle and move to the tool change position then wait for you to press cycle start before proceeding. That gives you the opportunity to do the tool change manually. This will work by either entering the T# M6 command into the MDI screen or in a program. My programs typically have 6 or 7 tool changes that are all done manually. Works great everytime

Hope this helps.

Cheers, Stephen Brown

 

[metzenovich]

Thanks for the info. I'll take a look.

I think I can write a quick post processor (post-post-processor, acutally, since I'll run it on the G-code after exporting the file from Fusion 360 and before running it on the Masso, using Python or something similar) that will replace the T# M6 lines with my own G-code to open and close the right valves in the right order to do the manual tool change with all the various steps for my ATC. It will still be manual, but will make the process faster and easier, and human error less likely.

 

[testyourdesign]

You might be able to use M62 / M63 option for what you're trying to do. Check out https://www.masso.com.au/masso-docu...rn-on-digital-output-synchronized-with-motion

Cheers, Stephen Brown

 

[metzenovich]

Quote from testyourdesign on February 10, 2020, 6:19 pm

You might be able to use M62 / M63

Thanks. That's what I was hoping.

Something roughly like this:

M5 (spindle off)
G01 Z0 (safe z)
G01 X0 Y0 (go home)
M00 (wait for cycle start)
M11 (open the drawbar)
M62 P1 (turn on the air purge)
M00 (wait for tool change / cycle start)
M10 (close the drawbar)
M63 P1 (turn off the air purge)

There will be more to it than that, but that's the general idea. Then I can use M98 / M99 to create include files for each tool change. I may need to include a T1 M6 command (even though I just press start to continue) as a way to show me on screen which tool to install. I don't know if there is a way to include a message on screen with an M00. If not it would be nice if any comment (or the entire line) on the M00 line showed up on screen. But I'll create a feature request for that separately if needed, after I actually get to that point.

Thanks

 

[breezy]

I would use

G28 G91 Z0.
G28 G91 X0. Y0.​

instead of

G01 Z0 (safe z)
G01 X0 Y0 (go home)​

Because your code would move to the WCS position not the home position. G28 is go home command and the G91 Z0 is MCS Z zero.

I think I can write a quick post processor (post-post-processor, acutally, since I'll run it on the G-code after exporting the file from Fusion 360

You could write the whole thing into the Fusion postprocessor. I just had a quick look at the MASSO postprocessor but couldn't find the section to use, will look again later and try to write the required code for your tool change to happen.

Regards,

Arie.

 

[breezy]

@metzenovich,

Found time to search Masso.cps and added your gcode to the postprocessor.

If you wish to further manipulate the processor code, search for

if (properties.useM6) { ​

This is the output that I created

(COMPRESSION CUT)
N35 T2 M6
N40 G28 G91 Z0.
N45 G90
N50 G28 G91 X0. Y0.
N55 G90
N60 M0
N65 M11
N70 M62 P1
N75 M0
N80 M10
N85 M63 P1
N90 S20000 M3​

The four lines after the tool change command are the safe retract, after that is the code that you alluded to.

You will need to setup MASSO for manual tool change without movement to tool change position. If you can't do that then we need to remove the safe retract commands as in the manual tool change MASSO retracts to the Z safe location and you tell it where you want the tool change location to be.

Hope this is helpful.

Regards,

Arie.

 

[metzenovich]

Quote from Breezy on February 11, 2020, 9:13 am

Found time to search Masso.cps and added your gcode to the postprocessor

Thanks, Arie! That's very kind of you. Not only did it help solve my problem, it gave me a guided tour through the Fusion 360 post-processor. That will come in very handy.

I'm waiting for a sensor to come in, then I can try it out.