[Donkey Hotey]

I've been asked to help move a process from a manual mill to our Multicam 3000 router / knife cutter. The machine uses fairly straightforward G&M codes. The main problem is the Z axis. The Multicam has a flipped Z-axis: positive values are down and negative is up.

I originally thought that I would copy the generic 3-axis mill definition and post, then alter from there. I thought that I would change the Z-axis direction in the Machine Definition and that would fix everything. I found that spot on the Machine Def, flipped it so positive Z was pointing down but, it still posts with positive values being up.

The question: where will I have to invert the Z-axis values? In the post? In the machine definition? Is this a setting somwhere else I hadn't thought of?

I already posted the output, used MS Word to search & replace all of the Z values into Z-. The output works fine except for this one glitch.

[Superman]

In the mastercam post, find the actual string holding the Z values and multipy by -1

A -ive Z will end up as +ive, and visa-versa

I'm thinking you may have to go to the "Motion output components"
and do the re-config here ( sorry, I'm not in a position to test it )

pfzout          #Force Z axis output
      if absinc$ = zero, *zabs, !zinc
      else, *zinc, !zabs

pzout           #Z output
      if absinc$ = zero, zabs, !zinc
      else, zinc, !zabs

[Donkey Hotey]

Thank you. That's helpful. I guess I don't understand what the role of the Machine Definition and Control Definition have in all of this. I've only recently started tinkering with the posts to get what I want out of them.

Where can I find a list of all of those program output names and their definitions? Yeah, I see them listed through the post but, I'm never sure which value is what output from Mastercam (pzout for example).

[Superman]

The way I understand the Mcam setup is basically

Machine definition file : calls up the post and control, sets the Max RPM, libraries, file paths, and all the other $hit that goes with it, and just ties them together under 1 specific machine banner

these files ( control & post ) can also belong to other machines, but the idea is to program the part then pick the machine you want it posted to, and everything needed is under that machine's heading

OK, post info.... have a look at your documentation & help directories, there may be PDF's about posts, editing, ( haven't got mcam at home ). But....There is one , I've seen it or was it V9 ??? with postblocks and so on.

Ping back if you can't find it, I'll try to find something on my side of the globe, got it stashed somewhere

[Superman]

You actually need to modify the variable that holds the value
the pzout & pfzout holds the address and value

I just did a simple contour, and the output seems to give what you need

pfzout          #Force Z axis output
      zinc=zinc*m_one, zabs=zabs*m_one # changes Z sign-added ST 27/4/2010
      if absinc$ = zero, *zabs, !zinc
      else, *zinc, !zabs

pzout           #Z output
      zinc=zinc*m_one, zabs=zabs*m_one # changes Z sign-added ST 27/4/2010
      if absinc$ = zero, zabs, !zinc
      else, zinc, !zabs