Official Luthiers Forum!
http://www-.luthiersforum.com/forum/

Question about Post Processors, ATC, and tool lengths
http://www-.luthiersforum.com/forum/viewtopic.php?f=10106&t=46033		 Page 1 of 1
Author:  Durero [ Thu Jul 16, 2015 2:13 am ]
Post subject:  Question about Post Processors, ATC, and tool lengths
I'm setting up my ATC functions on my CNC Router and I've never dealt with automatic tool changes or Post Processor files before.

My first test cuts not working just because the different tool lengths are not being used. Paths with different tools are being treated as if all tools are the same length.

I've set the tool lengths correctly in MadCAM and I strongly suspect that my problem lies in the Post Processor file and / or Mach3.

I don't have a Post Processor file specifically for my machine so I have to make my own. I've looked through the generic Post Processor file I'm using and added G44 (positive tool length compensation) or G43 (negative tool length compensation) but neither is having any effect.

I've also tried entering different tool lengths into the Mach3 tool table but no effect so far. Not sure if the tool lengths have been disabled somewhere else within Mach3.


Any suggestions would be very gratefully appreciated! :mrgreen:
Author:  rlrhett [ Thu Jul 16, 2015 2:43 am ]
Post subject:  Re: Question about Post Processors, ATC, and tool lengths
You might want to post some actual code. Nothing too long, but a short program with a couple of tools each making a simple linear cut that is causing you grief. Maybe we can see what is happening from there.
Author:  demonx [ Thu Jul 16, 2015 2:50 am ]
Post subject:  Re: Question about Post Processors, ATC, and tool lengths
I don't bother setting tool length in my cam, just the tool number, type and width.

My post processor doesn't have anything to do with the offsets or tool changer. Keep it simple.

I've found it much easier to set the tool offsets in Mach3. It'll override any offsets you create in your CAM anyway, so I don't bother to even set them.

I use my longest tool as tool 1. Then I set that as zero (on workpiece), then I'll move tool 2 to that zero (BUT DONT REZERO), in Mach 3 offsets page click "set tool offset" and then hit "save offsets", then repeat for tool 3, and so forth.

Do a couple of test tool changes and set your zero on something soft so that if its not right you don't wreck your cutter, keep your remote in your hand and be ready to hit stop in a hurry.

After you get the hang of it you'll be doing it second nature.
Author:  demonx [ Thu Jul 16, 2015 3:02 am ]
Post subject:  Re: Question about Post Processors, ATC, and tool lengths
You don't need to cut wood to know if your Mach 3 offsets are right.

Just zero tool 1 somewhere, then go to the MDI page in Mach 3 and type "T2 M6" into the browser down the bottom and hit enter, then hit goto zero. If it pulls up to your zero then the offset is right. Then T3 M6 to check tool 3 and so on.

Again, use something soft as a test surface as if your cutter dives deep and it's a small cutter, you can kiss it good bye! Once you're comfortable with how it all works then you'll be able to do it on s hard surface.
Author:  Durero [ Thu Jul 16, 2015 3:05 am ]
Post subject:  Re: Question about Post Processors, ATC, and tool lengths
Ah fantastic, I'll give that a try!

Thank you!!!
Author:  Sheldon Dingwall [ Thu Jul 16, 2015 12:29 pm ]
Post subject:  Re: Question about Post Processors, ATC, and tool lengths
+1 to all of the above. Set the tool offsets at the machine. ALWAYS assume you're going to mess it up if you don't concentrate 100% while doing this. If you misplace a decimal you could ruin your piece, cut into your vacuum fixture or even your table faster than you can hit the E-stop.
Author:  demonx [ Fri Jul 17, 2015 5:28 pm ]
Post subject:  Re: Question about Post Processors, ATC, and tool lengths
Did you get it sorted?
Author:  Durero [ Thu Jul 23, 2015 12:15 am ]
Post subject:  Re: Question about Post Processors, ATC, and tool lengths
I gave it a try today but the tool offsets are not taking until I manually press the "Tool Offsets Off/On" button twice.

The offsets are saved correctly between sessions.

I think I've got Mach3 configured to ignore tool offsets by default, or something wrong in my tool change program.

Next chance I get I'll dig around some more.

Really appreciate the suggestions so far.
Author:  demonx [ Fri Jul 24, 2015 5:59 pm ]
Post subject:  Re: Question about Post Processors, ATC, and tool lengths
Try this:

From a fresh startup, load your tool #1 (I have a dummy tool change set so that when I finish it unloads the current tool and picks up an imaginary tool)

If tool #1 is the tool all offsets are calculated from, the offset button-light will still be off.

Now get it to drop tool 1 and pickup tool 2. Mach 3 should automatically turn on the tool offset button/light now.

It's not something I turn in automatically. Mach does it. However this did confuse me at the start.
Author:  Durero [ Fri Jul 24, 2015 10:22 pm ]
Post subject:  Re: Question about Post Processors, ATC, and tool lengths
Thanks so much for all of your help Allan.

I finally got it working today by adding G43 with H(tool number) to my tool change program. I missed the H tool offset number in my previous attempts.

After that everything behaved just as you described.

On to the next challenge!
Author:  demonx [ Sat Jul 25, 2015 6:02 am ]
Post subject:  Re: Question about Post Processors, ATC, and tool lengths
No problem, glad you got it sorted.

I'll be needing some help soon enough when I get the funds together for a vacuum system, so I'll be in the same boat as you, trying to work stuff out!
Page 1 of 1 All times are UTC - 5 hours
Powered by phpBB® Forum Software © phpBB Group
http://www.phpbb.com/