fusion 360

General topics about everything that doesn't fit elsewhere.

fusion 360

Postby kenyoung » 17 May 2015, 21:01

I am new to cnc, I just finished building my cnc router and got everything working. Now I'm looking at the software end. I used the trial versions of meshcam and cambam then I found fusion 360 and found it a very powerful program, I created a simple plaque with recessed text and tried to open it but kept getting error messages. I went into the export window and found a choice for mach3 and even a choice for rs274 but kept getting error messages like unknown code line 2, beginning of radius different than end of radius ect. What am I doing wrong/ any suggestions, what export option should I choose in fusion 360 or will it even work. I could switch out the breakout board and run mach3 but I don't want to. I purchased the components from build your cnc but used my own machine design so the board is the diy version. Any help would be great.
kenyoung
 
Posts: 5
Joined: 17 May 2015, 20:25

Re: fusion 360

Postby Support » 20 May 2015, 07:34

Have you tried any post processor which name ends with a word "g-code"?
We don't really have any experience with this CAM sw...

You get errors because definitions for these g-codes are not supported in that form on our controller.
Support
 
Posts: 2571
Joined: 07 Apr 2014, 17:39
Controller: Many controllers

Re: fusion 360

Postby Marcos » 21 May 2015, 13:57

Look at this http://www.planet-cnc.com/forum/viewtopic.php?f=5&t=1346
Fusion 360 and Inventor HSM likely use the same .cps files which are the post processor definition file.

or just try out some of these .cps (emc gbrl mach2mill). Try to edit the resulting gcode, if there are problems, find out the one (.cps file) which comply at most and then:

This .cps files also can be modified with a text editor.

Please post your results, and what mods you applied. It should be possible to get a planet-cnc.cps file to share.
Marcos
 
Posts: 3
Joined: 13 Feb 2012, 16:33
Controller: Mk2

Re: fusion 360

Postby kenyoung » 05 Jul 2015, 19:44

By the time the post was moderated I had found that mach3 post processor worked for the most part only had to edit a couple of lines of code, mostly because I don't use the homing procedure on the machine, so "go to a predefined location" does bad things. Anyway thanks for the response, now on to the next challenge, I am trying to get some templates that I hand drew into a cam program. They are on 36"x 144" paper. I scanned them into the computer in pdf format, converted them to bump but they are just too big for meshcam to handle. Any suggestions? I converted them to J peg and will try and separate the individual template's.
kenyoung
 
Posts: 5
Joined: 17 May 2015, 20:25

Re: fusion 360

Postby Allen McFarlen » 06 Jul 2015, 19:44

If you are using Fusion 360 then you can import them into a new document as a canvas and create new sketches over them.

There are plenty of tutorials on YouTube showing the procedure for Fusion. I've done it with many of my templates that were drawn up in various other programs over the years.
Allen McFarlen
 
Posts: 39
Joined: 25 Mar 2014, 00:19
Location: Cairns, Australia
Controller: Mk3

Re: fusion 360

Postby garethky » 28 Aug 2015, 08:00

I've used the Mach3 post processor to run a couple of parts. So far its working well.

The only issue I have with the resulting G-code is that at the start of the program the tool is not moved up to the clearance height. So the initial traversal that happens can mar the stock. After that it will retract to the clearance height between operations. The programs also traverse back to the G28 stored position at the end of the program, with z-height at the G-28 height, not the clearance height.

Generally we set the tool on the stock to start to get a good 0 point reference and then set G28. I'm still looking for a workaround. The post processors are all in Javascript so modifying one is possible.
garethky
 
Posts: 4
Joined: 10 May 2015, 06:59
Controller: Mk2

Re: fusion 360

Postby garethky » 14 Sep 2015, 04:07

I was able to tweak the Mach 3 post file to fix the issue I was seeing. See attachment (just re-name it to planetcnc.cps to use it. The forum wont let me upload .cps files).

Looks like Autodesk has a pretty standardized post processor file with some parameters they can tweak. Its all in Javascript which is nice. Anyway...

The standard program end is the following instruction sequence:
G28 Z0.
G28 G91 X0. Y0.
M30

This first returns the Z axis to 0 of the machine offset (G28 position). Then it moves in the X and Y to the machine offset position. This seems all kinds of wrong. :? The exact opposite of the "Go To - Zero" function in Planet CNC.

Usually we touch the bit to the work surface to set the offset potion ('Set Position - Zero' in the PlanetCNC menu). And Fusion is good about writing programs that retract the tool and do all rapids between operations at the defined retract height. The program end sequence should honor this as well. So I just revered the lines of code involved and now it spites out:

G28 G91 X0. Y0.
G28 Z0.
M30

I don't know what the legal status of the file I modified is. Since it started out as an Autodesk file I have left their copyright header intact. But they seem to want third party developers to work on post processors. They have a manual that covers it: https://autodesk.app.box.com/s/3zk4u2tyr1v4oaphscog

@Support, how do you feel about this, maybe as a github project?
Attachments
planetcnc.cps.txt
(32.05 KiB) Downloaded 211 times
garethky
 
Posts: 4
Joined: 10 May 2015, 06:59
Controller: Mk2

Re: fusion 360

Postby koscielniak » 25 Sep 2015, 01:17

I too use Fusion 360 at home and Esprite 2015 at work. Fusion is incredibly powerfull CAD/CAM for most things. I use the generic Hass mill post for my home built machine as it does not kick out any unnecessary code that my home built machine can not support.

koscielniak
koscielniak
 
Posts: 7
Joined: 24 Sep 2015, 00:21
Controller: Many controllers

Re: fusion 360

Postby dudemeister » 02 Feb 2017, 19:49

Thank you for attaching these posts files. I was at a loss on how to implement Fusion 360 post processing into the Planet CNC software. No issues importing gcode now. Thanks again.
dudemeister
 
Posts: 10
Joined: 14 Dec 2016, 05:47
Controller: Mk3


Return to General topics



Who is online

Users browsing this forum: No registered users and 1 guest

cron