Machsupport Forum

Mach Discussion => Mach4 General Discussion => Topic started by: homebuilt on February 15, 2019, 06:44:32 PM

Title: Mach 4 and fusion 360
Post by: homebuilt on February 15, 2019, 06:44:32 PM
Hi guys just wondering if anyone might be able to help.

Fairly new to this but ive got everything up and running in metric motors tuned and accurate etc etc but i make a simple object in fusion 360 do the CAM with toolpaths and save the file.  I import it into MACH 4 and everything is just a huge line or just none existent i cant seam to find anywhere to bring the file into the file into the tool path window like all the videos i have watched and cant for the life of me work out what i have done.

Ive added the fusion file below if it helps its just honestly a 100x100m square with 2 holes in it and its driving me insane

thanks again i love coming onto the forum and learning :)

Title: Re: Mach 4 and fusion 360
Post by: joeaverage on February 15, 2019, 06:55:25 PM
I see the code has a G71 near the top of the file:

Code: [Select]
: (PGM, NAME="2001")
; T5  D=4 CR=0 - ZMIN=-17 - FLAT END MILL
: G90 G40 G94
:T5 M6
S5000 M3

A G71 command should set the units with which the file is to be interpreted as millimeters. If you look in the 'Mill Gcode
Programming' pdf in Mach4s Docs folders there is no entry or description of G71. G71 IS described and supported in
Mach3 but not, to my knowledge in Mach4. In fact G71 is old school and I believe is deprecated in ANSI Gcode as well.

May I suggest editing the G71 to the currently supported G21 and try the code again.

If its effective you may need to tweak the Fusion Post to use G21 rather than G71.

Title: Re: Mach 4 and fusion 360
Post by: homebuilt on February 15, 2019, 07:53:11 PM
Hi I've cut and paste the code into the MDI ( not sure if that's the right thing to do and change the g71 to g21 and regenerated the code but in the window it has come up with a strange shape that's not even close to what I was wanting I've attached a photo
Title: Re: Mach 4 and fusion 360
Post by: joeaverage on February 15, 2019, 08:20:52 PM
you now at least have it operating in mm.

Now you have Mach operating in one arc mode whereas Fusion is producing code in another mode.

Change the mode of Machs arc interpretation to check it out.

Thereafter it will be necessary to change the Fusion post to generate compliant code.

Go to Configure/Control/General and change arc center mode from Incremental (normal) to absolute.
Run the code again. If it pans out there are instructions in the Fusion forum about changing the post.

Title: Re: Mach 4 and fusion 360
Post by: homebuilt on February 15, 2019, 08:47:08 PM
Hi Craig changed to absolute in arc centre mode but I'm not sure what I'm looking for in the fusion forums to make it work together.

I also have the error " K word given for arc in xy plane" and that's got me stumped also
Title: Re: Mach 4 and fusion 360
Post by: joeaverage on February 15, 2019, 09:04:08 PM
I have used Fusion briefly. You will have to find out more from the Fusion guys but as it stands Fusion is
producing bad code.

Title: Re: Mach 4 and fusion 360
Post by: homebuilt on February 15, 2019, 09:07:51 PM
Would you recommend anything that might be better or something I can use for comparison Craig?
Title: Re: Mach 4 and fusion 360
Post by: joeaverage on February 15, 2019, 09:23:41 PM
Fusion is used and recommended by plenty of users.

For all that I am dubious about Autodesks motivations about Fusion I can still only complement their commitment
to their stated aims.

If you are prepared to stick with it and get a good Mach4 Fusion post you will be good.

The only other suggestion I have is to use Mach Mill wizard. It produces good code and is very useful for chains
of usefull machine operations. I use commonly for chainging simple operations together to create a Gcode job WITHOUT using
a CAM program at all. It costs $75 USD.

Title: Re: Mach 4 and fusion 360
Post by: thosj on February 16, 2019, 09:01:52 AM
Are you milling or turning? You mentioned a square with holes so I assumed milling.

Google shows G71 as a Fanuc turning gcode, not a G21/G20 alternative. That M26 in your gcode is a little odd, too,

Perhaps, even LIKELY, I misunderstand your dilemma:)

What Fusion post are you using?

Title: Re: Mach 4 and fusion 360
Post by: joeaverage on February 16, 2019, 03:57:50 PM
Tom is right, m26 seems misplaced.

Note also the spattering of g17 and g18's throughout the code. g17 declares the machining lane as xy whereas
g18 declares the machining plane as xz.

The link that Tom posted suggests that m26 is somehow related to lathe operations and the g18 seems to confirm it.

Could it be that Fusion is generating code for a lathe not a mill?

If I understand your situation you are new to Mach4 and possibly even CNC? If that is the case you have too many
'variables' going on. Mach4 in itself takes a little learning, using faulty code is making that learning impossible.
Likewise Fusion takes a lot of learning as well, but worse is that you clearly cannot read Gcode nor are you confident
of the machine software.

May I suggest ditch Fusion.....for the moment. What you need is good Mach compliant code that you can run through your
machine so you can gain familiarity and confidence in it. You also need to start to read Gcode. There are many online
tutorials about Gcode. You don't need expertise in Gcode but you should be familiar with what good code looks like.

For that purpose you should be writing Gcode manually or using a wizard. My recommendation is Mill Wizard.
Download it for free and experiment with it. You should be able to produce goo Gcode for simple operation in
under half an hour.

As an example about a week ago I had to machine a heatsink for a electronic project I'm working on. The material
(extruded finned heatsink) had previously been used. I required that the top face be surfaced and then four rectangular
pockets be formed. I stood at my machine for about 5 minutes and had Gcode, and about another 5 or 10 using s Gcode
viewer to verify and fine tune it before running the job. I had four heatsinks to do, it took 20 minutes to machine all

This is an example of simple jobs that don't require a CAM program. You may have seen advertising material for Fanuc, Hass,
and Siemens and they both bang on about 'conversational programming' It is exactly the process I have just explained.
It allows a machine operator to stand at the machine and in short order chain together simple machining ops
all WITHOUT using CAM. This allows a machinist to be highly productive despite not be a programmer.

Of course there is a place for CAM programs as well. They typically are used in the office and then given to the operator
to run on the machine.

Title: Re: Mach 4 and fusion 360
Post by: TommyG on February 18, 2019, 05:13:42 AM
I regularly use Fusion 360 with Mach4 and it works fine. As the posts above state you probably have the wrong post processor selected.

Some instructions below on how to select the correct post processor but I would add that some of the advice above is very good. I'd particularly echo Craig's (joeaverage) advice that if you're totally new to Mach4 and CNC then Fusion 360 is going to add a layer of complexity you probably don't need or want. I like it for CAM but it took me some time to get my head around its peculiarities, it's certainly not as intuitive as other programs I've used.

To select the CAM processor

Go to and search for Mach4Mill. Download that post processor to somewhere on your computer. I'd suggest creating a folder in the Mach4Hobby directory, something like C:\Mach4Hobby\Fusion360Posts. You're better clicking on the "Download" button rather than opening the file and copying the contents, you avoid issues with different types of newline characters between different OSes that way.

In Fusion360, when you select "Post Process" in the CAM workspace, change the "Configuration Folder" to point at the location above. The "Post Configuration" should automatically change to "Mach4Mill / mach4mill" assuming it's the only post processor in the directory. That should be you good to go.

You're also better opening the gcode file in Mach4 rather than copy and pasting the contents to the MDI window, that can also cause the issue with newline characters being mixed up and result in the single line issue you noted above. Windows Notepad (up until the very newest versions in the latest builds of Windows 10) is a particularly bad offender when it comes to this.

Hope this helps

Title: Re: Mach 4 and fusion 360
Post by: Cbyrdtopper on February 18, 2019, 05:30:33 PM
I'm with TommyG, I use Fusion 360 with Mach4 all the time.  I would check the post processor like he has suggested.