topic How to choose G55 work coordinates in Fusion Manufacture Forum

How to choose G55 work coordinates

SGoldthwaite — Sun, 26 Apr 2015 22:15:06 GMT

In my gcode I want to use G55 instead of G54. How do I configure this in Fusion 360 CAM?

Re: How to choose G55 work coordinates

fonsecr — Sun, 26 Apr 2015 23:26:33 GMT

In the Setup you can choose the "work offset" which by most posts and ISO posts in particular is used for the G54, G55, and so on.

By convention, work offset 0 means use the default one (which is G54 for ISO posts). Value 1 is the first one G54, value 2 is the second one G55 and so on. Having 0 as the default ensure that it works for posts/CNC which do not have a work/fixture offset concept like normal ISO CNCs.

Re: How to choose G55 work coordinates

Anonymous — Mon, 19 Oct 2015 19:16:17 GMT

Quick question on multple coordinates in one setup. I sometimes use Sprutcam and an operation can be assigned a coordinate system. The resulting single G code file contains all of the code for all operations. As a user you need to know to change the coordinate system at the Mill. Tormach demonstrated this in one of their training sessions. I just started using Fusion and with multiple setups it's easy to assign coordinates. Also each has it's own G code file. I just made a new project and it has only 1 setup. Within this setup there are several operations. In each operation I set the tool orientation appropriately for the maching to be done. When generating the post process it fails. Looking at what little code was written I see that it fails just after a couple lines of the operation with a new coordinate system. G54 is one the first operation but seems that it fails just after an M30 line. I tried several reorders of the operations just to test it and it still fails anytime there is a coordinate system change.

Any thoughts for a newbie?

Thanks. I also understand your 0/1 2,3 G54, G55 etc. numbering.

Re: How to choose G55 work coordinates

HughesTooling — Mon, 19 Oct 2015 19:25:07 GMT

Are you getting a warning log file, if your editor is Brackets I'd change to notepad as it picks up the warning file more reliably. To change go to Properties - General - CAM and change the editor to notepad.exe and try posting again. Also can you Export the file as f3d and attach here please.

Mark

Re: How to choose G55 work coordinates

Steinwerks — Mon, 19 Oct 2015 19:25:09 GMT

Unless you're using a 4th axis rotary, I wouldn't try and use Tool Orientation, it will not work. You CAN output multiple setups in one file, but the post may need tweaking to get it to do what you want.

Re: How to choose G55 work coordinates

fonsecr — Mon, 19 Oct 2015 19:28:37 GMT

The work offset is what maps to G54, G55, G57, and so on.

The actual coordinates will be output in the WCS coordinate system that you have chosen for your Setup. If you use a different Z orientation in an operation you will effectively be doing multi-axis indexing toolpath. Which your post then needs to support or it will fail saying that it cannot reach the orientation selected.

The WCS corresponds to the physical placement on the CNC. And whenever you change the physical placement you need to use a separate Setup.

René

Re: How to choose G55 work coordinates

Anonymous — Tue, 20 Oct 2015 00:35:43 GMT

Getting closer but now need to know how to change to G54, 55, 56.
Answer in link below says to select multiple setups and Post them to one file. That works so far. Now I need to confirm how to change coordinate system after moving part.

https://camforum.autodesk.com/index.php?topic=8007.0

I see a G54 in the first lines of code but no G55 or G56.... anywhere in the code. I think I may have to tell my mill. Does anyone have an answer for this? Modify GCode??
Thanks.

Re: How to choose G55 work coordinates

Anonymous — Tue, 20 Oct 2015 00:48:37 GMT

Sorry I didn't see your answers before my last post. I can select multiple setups and post successfully. I just finished that and don't see any other G5x lines in the code. Do I need to modify the G-code to set G55, 56 or, based on some other posts, it will know what coordinates to go to? I will try tomorrow a test run without tool or spindle. Any other comments are greatly appreciated.

thanks

sorry for my missing your replies earlier.

Re: How to choose G55 work coordinates

Anonymous — Tue, 20 Oct 2015 00:50:47 GMT

Here's the archive file. It's just a practice drawing.

Re: How to choose G55 work coordinates

Steinwerks — Tue, 20 Oct 2015 01:10:40 GMT

Right click on your setup, go to Post Process tab, select WCS Offset (G55 would be 2).

Re: How to choose G55 work coordinates

fonsecr — Tue, 20 Oct 2015 07:53:48 GMT

PS. The generic posts will by default only output G5x when they change.

The convention is for work offsets for the ISO posts are:

0: default (aka G54) (this is because 0 is used as disabled for certain CNCs)

1: G54

2: G55

3. G56

4. ...

René