Need some help with a UMC-750 post for Fusion.

I had a message asking me for some help from someone in the Haas group using Fusion on a UMC. He sent me a sample of the code and right off the bat there's issues with the post or settings, Im guessing both. I only tinkered with Fusion when it first came out then dumped it so I have no clue how to get this kid up and going with post mods.

For some reason its throwing out a G53 after the G54 call (Damn that could get ugly. Then in the middle of the feeding it swaps plains (G18 to G17 , That could get real ugly).

Its apparent that the kid cant read code and apparently he don't want to tell his employer so i'm trying to help him out a little before he crashes someone else's machine.

If someone on here has a post they are using or knows to be good for a UMC I would appreciate a copy.

[email protected]

is it the post on Fusion post site that you started with?

Post Library for Autodesk Fusion 360 | Autodesk Fusion 360 then go to vendor and pick HAAS

The G53 line is a positioning move to a safe position in machine coordinates for rotary positioning, and a Z retract is omitted because the post knows a tool change has just occured. G53 is modal for its block.

G18's are from the vertical lead in arcs.

In terms of code syntax, there doesn't appear to be anything wrong.

The G53 line is a positioning move to a safe position in machine coordinates for rotary positioning, and a Z retract is omitted because the post knows a tool change has just occured. G53 is modal for its block.

G18's are from the vertical lead in arcs.

In terms of code syntax, there doesn't appear to be anything wrong.

Click to expand...

The N40 G53 machine co ordinate cancels the N35 G54 work coordinate. I'd say there's something wrong.

g-coder05 said:

The N40 G53 machine co ordinate cancels the N35 G54 work coordinate. I'd say there's something wrong.

Click to expand...

As goofy as that code looks, there doesn't seem to be anything wrong. G53 does not cancel G54. G53 is a "one shot" G code working off the Machine Coordinate System. G54 is again the relevant offset in the block following without calling it again because it is Modal. (See below.) For whatever reason his fist move uses G53. Perhaps a known safe zone to Fusion in the current setup. You'll notice he positions again and activates the tool offset later. I'm not familiar enough with 4 or more axis mills to comment about a lot of the other stuff going on.

CJ said G53 is "Modal to it's block. I'd like to suggest that that is poor usage of the word modal. Every G or M code or piece of text or code of any type is in that usage "modal" to the block it's in, which sort of doesn't make sense. Try using "one shot" G code for G53, or something along that line. I think that is the standard terminology for it though I could be wrong.

Dave