Hello Guest it is February 28, 2021, 07:59:27 PM

Author Topic: Fusion 360 Mach 3/4 Post Processing Configuration  (Read 898 times)

0 Members and 1 Guest are viewing this topic.

Fusion 360 Mach 3/4 Post Processing Configuration
« on: September 08, 2018, 11:35:47 AM »
As the title suggests, i'm trying to modify the way Fusion 360 posts with Mach 3/4 post processor from Autodesk HSM.
One problem i've encountered is  zeroing Z axis and loading a program into Mach 4. Starting the program, Z tries to home itself instead of running the program. I have to reset Z and then it will run correctly once started. I've remove M6 tool change as i thought that might be causing the issue. It didnt help. The following is a sample of the g-code from Fusion and then an example of it modified. What am i missing? Also, I am setting up to run as a individual part without g54 or fixturing. I manually set all axis and run from a set point on material or edge of material. Mostly run 1/2" 6061 plate and under, clamped to table with a sacrificial plate.

Fusion Post-

(7002)
(HEADSTOCK BACK SHIM)
(T1  D=0.25 CR=0. - ZMIN=-0.25 - FLAT END MILL)
G90 G94 G91.1 G40 G49 G17
G20
G28 G91 Z0.
G90

(BORE1)
M5
M9
T1 M6
S1400 M3
G54
M8
G0 X4.2713 Y1.7887
G43 Z0.6 H1
Z0.055
G1 Z0. F6.
Y1.7762


And my mods -

(7002)
(HEADSTOCK BACK SHIM)
(T1  D=0.25 CR=0. - ZMIN=-0.25 - FLAT END MILL)
G90 G94 G91.1 G40 G49 G17


(BORE1)
M5
M9
T1
S1400 M3
M8
G0 X4.2713 Y1.7887
G43 Z0.6 H1
Z0.055
G1 Z0. F6.
Y1.7762

Any ideas? Progams run fine except for needing the resetting of Z.
« Last Edit: September 08, 2018, 11:38:01 AM by rodm717 »

Offline Stuart

*
  •  244 244
    • View Profile
Re: Fusion 360 Mach 3/4 Post Processing Configuration
« Reply #1 on: September 08, 2018, 12:07:12 PM »
Where are you setting the WCS in fusion 360 setup in cam , that’s where you set the WCS on the mill

Usually the corner of the stock

The g28 in the code you do not like is easy to get rid of when you post out in fusion360 drop down the prefs and untick the use g28 box
Re: Fusion 360 Mach 3/4 Post Processing Configuration
« Reply #2 on: September 08, 2018, 01:47:25 PM »
Rodm717,
Stuart is right, turn off G28 when you post the code.
Fusion Posts the Code to make the Z go to Machine 0 for clearance purposes at the beginning of the program, every tool change, and at the end of the program. 
Turning off G28 makes the Z Retract plane for your machining operation the Z end point for tool changes and/or the end of program Z move.   

Also, you have to set up a Work Offset, otherwise your machine has no idea where to cut.  Like Stuart said, wherever you're setting up your WCS in Fusion is where you need to set your Work Offset on your machine. 
G54 is the default so that is what you set your X,Y, and Z 0.00 to. 
Chad Byrd

Offline Stuart

*
  •  244 244
    • View Profile
Re: Fusion 360 Mach 3/4 Post Processing Configuration
« Reply #3 on: September 08, 2018, 01:50:57 PM »
Thanks for the expansion Chad

I have difficulty in long explanations , I know what to do but my dyslexia plays up and I cannot get it down , paper and pencil is impossible

Re: Fusion 360 Mach 3/4 Post Processing Configuration
« Reply #4 on: September 08, 2018, 01:54:52 PM »
I Got you Stuart!  =) 
I like how you explain things, straight to the point.  I just happened to have a picture of all this so I decided to post it. 

Also Rodm717,
It isn't that difficult to edit your post processor.  I always take out the G28 X move, because I don't want my machine to move the X all the way over.
Now, if you want to get crazy technical and edit your post processor; you can do this.  
John Saunders has some awesome videos for Fusion 360. Here is one:
https://www.youtube.com/watch?v=OJO_u7XjVHg

I plan on doing this to 1 of my post processors for 1 machine I run in the shop.  
Chad Byrd
Re: Fusion 360 Mach 3/4 Post Processing Configuration
« Reply #5 on: September 08, 2018, 02:59:17 PM »
Where are you setting the WCS in fusion 360 setup in cam , that’s where you set the WCS on the mill

Usually the corner of the stock

The g28 in the code you do not like is easy to get rid of when you post out in fusion360 drop down the prefs and untick the use g28 box

Thanks. Dead on. I didnt realize g28 was a built in setting in Fusion post. Yes, i work off corner of  model.
I've tried all kinds of things and the elimination of G54 was a oversight/error on my part.
I'm still working on figuring out a config that will work for various setups and haven't played with fixture in program or offsets.
I'm leaning towards purchasing a probe. I guess that will also bring another set of things to solve, but should help with almost any situation.
Re: Fusion 360 Mach 3/4 Post Processing Configuration
« Reply #6 on: September 08, 2018, 03:52:28 PM »
http://www.machsupport.com/forum/index.php/topic,37808.0.html
Here is a thread that discusses Work Zeros.

What do you mean by various setups?

Check out Artsoft's Youtube Channel.
https://www.youtube.com/watch?v=0aRifYB70Mc&t=42s
Chad Byrd