Manual tool change - Generic FANUC post

[bellman]

I have a small VMC with a chinese controller fitted. The controller uses FANUC mill as its post processor.

I have "manual tool change" selected in the tool library post processer tab.\

When I post the file using "Generic FANUC" the code has MO6 for the tool change which sends the machine to the tool-change position but the machine does not pause to allow a manual remove and replace of the tool. I have to edit the code for MOO after every MO6.

Should I be doing something differently, use another post or is this an error in the Generic FANUC post?

Thanks in advance for any help

Greg,

Australia

[Steinwerks]

The post needs to be modified to output an M0 in a tool change since it's a manual change. The post assumes that you have an ATC.

You will have to add a COMMAND_STOP somewhere, but I'm not knowledgeable enough to know exactly where to put it. I expect Hughes Tooling will be here soon though 

[HughesTooling]

Hi Greg

Here's the line that needs changing, there's only one mFormat.format(6) so it's easy to search for. Are you using a Mac or PC, it's a lot easier to edit posts on a PC.

If you're on a PC, on the post dialog click Open config and the postprocessor will open in your editor after editing you need to save to a different directory. One option is to save to Documents then follow my instructions in the thread to load the post to your cloud folder. One thing to note make sure you use a zero and not a letter O like you have in your post.

Mark

[bellman]

Mark,

Thanks for the help. I have found the file and renamed it, changing what I can but I do not know the correct syntax to add the COMMAND_STOP as suggested by Atomkinder67. If you wouldnt mind could you advise the line if code I need to add and should it go directly underneath the (6). I have searched DrGoogle and youtube for help on syntax but could not find anything able to steer me in the right direction.

Thanks for finding the mistake of MO (letter O) when it should have been zero.

Thanks in advance for any help given.

[HughesTooling]

Hi Greg

Just inserting   writeBlock(mFormat.format(0));  on the next line should do the trick, like this.

Make sure you don't save back to the generic post folder because it's moved every time Fusion updates, any non standard post are left in the old folder.

Mark.

[scottmoyse]

Enabling Optional stop in the post processor dialog may give you what you need anyway. By default if you hve the optional stop button active on your control, it will stop the machine right before the tool change.... it will just do it for every tool change.