Fusion Post Processor Questions

Post anything you want to discuss with others about the software.

Fusion Post Processor Questions

Postby Gadget » Sun Dec 31, 2017 5:53 pm

I got an error today when posting.
It seems lite it is due to my tool number being to high, in this case #200.
Is it possible to change this in the post processor and if yes, how?
I use Fusion mainly with my Tormach PCNC770 so I have reserved the first 200 tools for this machine.

Next question
When I post my file the pp adds a line "G43 H1".
Can anyone explain what that is and why it is there.
Is it possible to save a "Safe position" other than max z height?
As for now the machine goes to top z position before and after the program.
Posts: 13
Joined: Fri Dec 22, 2017 9:54 am

Re: Fusion Post Processor Questions

Postby skrap » Sun Dec 31, 2017 11:21 pm

This is from the UCCNC manual:

The tools page contains a tools table where there are 96 tool slots listed on 2 tab pages. The
different tools length can be programmed on the screen. The different tools can be selected
programming G43 H"tool number" or G44 H"tool number" in program or via the MDI. When
programming the G43 or G44, the tool length of the selected tool will be offset to the Z-axis. The
tool offset can be cleared programming G49 in program or via the MDI.

Have you tried a tool number above 96 (other than 200)? I don't see anything in the post processor that would care.

That section from the manual should also answer the question about what G43 H# is. So in your example it was programming a z-axis offset for the height of tool 1.

Where would you like it to go instead of Z0? Looking at the post processor it moves to Z0. You could change the 0 to whatever number you like. There are two lines in the post processor:

Code: Select all
writeBlock(gMotionModal.format(0), gFormat.format(53), "Z" + xyzFormat.format(0));

That commands the machine to make a rapid, absolute move to Z0. I'm unsure of undesirable impact of changing from Z0 to some other absolute position.
Posts: 18
Joined: Tue Apr 04, 2017 4:28 am

Re: Fusion Post Processor Questions

Postby Gadget » Mon Jan 01, 2018 12:03 am

Ok, I am used to tool being referred to as "T" and not "H".
Regarding the tool number, just as you say it is not possible to have a tool number higher than 96 (or 99?) without having an error.

"var lengthOffset = tool.lengthOffset;
if (lengthOffset > 99) {
error(localize("Length offset out of range."));

The problem with the offset is that z goes to 0 (MCS) no matter where the z0 (WCS) is.
It is not a huge problem, more a waste of time to have it go all the way up before and after a program.
On the Tormach/Pathpilot there is an M30 offset that lets you specify the "safe" z height between operations, tool changes etc.
Posts: 13
Joined: Fri Dec 22, 2017 9:54 am

Re: Fusion Post Processor Questions

Postby cncdrive » Mon Jan 01, 2018 12:27 am

Ok, I am used to tool being referred to as "T" and not "H".

The tool number of the tool length offset with G43 refered as the H parameter also in the Tormach: https://www.tormach.com/g43_g44_g49.html

The G43/G44 applies the tool length offset of the tool defined by the H parameter.
Selecting a tool is different, that is really done with the T word and it is adviced to use the M6 afterwords to switch the tool.
The M6 should contain your tool change routine/code if you doing automatic toolchange.
And it is not a mandatory to have the same tool length offset applied as what tool number is selected.

Tool lengths can be set on the tools page on the screen or you can upload the tool length table with G10 L1 if you want to set them programmatically.

And currently the UCCNC has a 96 size tool table, using larger tool numbers is not possible.
Site Admin
Posts: 1728
Joined: Tue Aug 12, 2014 11:17 pm

Re: Fusion Post Processor Questions

Postby spumco » Mon Jan 01, 2018 6:44 am

If you're using the "Generic UCCNC" post processor for F360, then you will get an error if any of the tool numbers in the output file are greater than 96.

A work-around is to leave your F360 local/cloud tool library tool numbers as-is, however you have them. Right before you post, open the tool library and select the current project. Re-number the tools to those matching the UCCNC tool table (assuming you've already set the tool lengths in UCCNC) and post the file.

Your local and cloud library tool numbers won't change - so they don't mess up anything for your Tormach - but the file you output will be compatible with UCCNC and the post processor won't throw up.

In fact, I use this as a 'safety' feature. All my tools in the local/cloud library are set to >100, which gives (forces) me one last chance to double-check the tool variables (F&S, size, mist/flood, etc.) before posting since I have to change everything for that program to a tool number that UCCNC will accept. It's another step in the process, but a fairly quick sanity check. If I had programs with 20 tools it might be a pain, but I haven't run a single program file with more than about 10 tools yet.

Posts: 151
Joined: Mon Oct 03, 2016 10:10 pm

Re: Fusion Post Processor Questions

Postby Gadget » Mon Jan 01, 2018 3:10 pm

It is all a bit confusing at the moment but I am sure it works out once I get used to the software.
As for now I haven´t entered any tool offsets but I have just ordered a tool length sensor so I might be back
with more questions soon.

Thanks for the help so far.

Best regards
Posts: 13
Joined: Fri Dec 22, 2017 9:54 am

Return to General discussion about the UCCNC software

Who is online

Users browsing this forum: No registered users and 2 guests