As I am aPh.D student I am enjoying the free version of Autodesk's Fusion 360. It is a very powerful CAM-CAD tool and easy to learn/use. I have created the gcode with the software as grbl generic. The software can post in many other formats too. My question is has any of you tried Fusion gcode with your builds? I want to decide what direction to go in for CAM software as I am a newbie. Following is a simple gcode created from Fusion for your reference. How do you interpret it? Does it look OK to you? There are too many options/parameters to choose from within the software and I believe it might be an option for us home users/students. Thanks % (1) (T1 D=4 CR=0 - ZMIN=-0.5 - flat end mill) G90 G94 G17 G21 G28 G91 Z0 G90 (Delikler4mm) M9 T1 M6 S16000 M3 G54 M9 G0 X27 Y21.5 Z27 Z12 G1 Z-0.5 F838.6 G0 Z12 Y13.5 G1 Z-0.5 F838.6 G0 Z12 X35.5 Y5 G1 Z-0.5 F838.6 G0 Z12 X43.5 G1 Z-0.5 F838.6 G0 Z12 X52 Y13 G1 Z-0.5 F838.6 G0 Z12 Y21 G1 Z-0.5 F838.6 G0 Z12 Y101 G1 Z-0.5 F838.6 G0 Z12 Y109 G1 Z-0.5 F838.6 G0 Z12 X43 Y118 G1 Z-0.5 F838.6 G0 Z12 X35 G1 Z-0.5 F838.6 G0 Z12 X27 Y109.5 G1 Z-0.5 F838.6 G0 Z12 Y101.5 G1 Z-0.5 F838.6 G0 Z12 Z27 M9 G28 G91 Z0 G28 X0 Y0 M30 %
I have recently been using Fusion 360 for CNC and 3D printing. I am still getting the hang of the CAD after using Sketchup for several years. The learning curve is steep, but once you get used to the process and learn some short cuts it works well. I really like being able to develop parametric models, so I can change material thickness later and the model adjusts. Very slick and powerful. Just today I needed a quick design to 3d print and used Fusion360 instead going back to my old standby (Sketchup). The CAM is working well for me. I am using a Tinyg on my OX CNC. Not sure on your gcode. Did you run the simulation in Fusion 360? You could try running it on a gcode viewer.
I'm a fan of f360. The support has been incredible on Autodesks part. Sculpt is super fun to use. I wish SW had sculpt. It would make the day job even better.
I built my first cnc (C-Beam) last weekend, using grbl(arduino) with cheap stepper drivers and grbl panel to send the gcode. I built my first design using Fusion 360 yesterday. I know absolutely nothing about cnc, and this was my first cut. I was able to fumble my way through the design and tool path creation process using the basic Fusion 360 videos from their site. When creating the gcode, I selected grbl generic and saved the file. When I tried to run the gcode file in grbl panel, there was an unsupported command error (I think it was T1 M6). I found the command and removed it from the file, and the cut went off without a hitch. So I can tell you, from a complete newbie standpoint, that you can use Fusion 360 gcode after you remove unsupported commands. I learned quite a bit during the whole process, like I should go back and add in a finishing pass ... And here is my first cut
Yes, soon I will start my experiments with cutting directly with Fusion 360.. I love the simulation before you go to the machine. It looks very promising and not so difficult to learn.. Thanks for sharing your experience @Jerry Ellis
After a few more projects, I found another trick. When I set up my material to cut, I zero the cutting tool on the surface. Fusion 360 produces gcode that will drag my tool across the surface to the location of the first plunge, then raises on the Z axes, and then plunges back down. Im sure there is a reasonable explanation for this behavior, I just dont know what that is The quick fix is to replace "G28 G91 Z0" with "G0 Z10" in the first few lines of the gcode... (THIS IS METRIC!!! If youre using inches, make the Z value something more reasonable!) This will raise the Z axis 10mm before it heads for the first plunge.
I am not currently at home where 360 is installed but I remember a setting for Z clearance. When defined, it should move your Z axis to that setting (e.g Z10) each time before your tool travels Y or X direction except while following the toolpath, created to cut.
I know there are settings for each tool path (clearance, retract, etc... ), but I couldnt find anything for the initial move from origin to the first plunge operation. If you figure out the proper way to do it, please let me know.
if you simply jog your machine, or home it and start at machine 0,0,0 it will return to work 0 with a raised Z.
Have a pock around in the "passes tab". This is just one of the many online videos that might help you, just play around in the software. Fusion 360: CAM for Intermediate and Advanced Users
Wow these videos are great. Does anyone have recommendations for C-Beam speeds, feeds, and DOC for pine, aluminum or acrylic? So far I have only run my machine flat out with a 4 flute end mill cutting some scrap plywood.
You may have just saved me a LOT of heartache! Ive been struggling with this all DAY EDIT: it worked! THANK YOU!
G28 causes this problem for me as well. I spent a lot of time trying to track down the problem and I found a few posts (including this one) that mentioned the G28 line as the problem. You can try disabling G28 by opening the generic grbl setting or you can download another config setup available on the post library. I used the following steps to download another setting grbl setting and get my machine to work correctly. 1) In Autodesk Fusion 360, go to CAM, then post-process. Under configuration folder, choose setup and select Online Post Library. 2) In the Online Post Library, search for grbl. At the bottom, you will see settings created by Inventables that have G28 disabled. Save one of the files. 3) Upload the file to your Autodesk folder. 4) In Autodesk Fusion 360, go to CAM, then post-process. Under configuration folder, choose setup and select Use Personal Posts. You should see the file show up under Post Configuration. Click Post. 5) In your G code sender, set your zero on your machine. Then lift the bit off the material to the clearance height (maybe 5mm). Then open and send the file. Hopefully, you won't see the machine drag across your work again.
G28..... G28 is supposed to be set to a safe position. If your machine homes with Z up away from the work like it is supposed to, then G28 will be a safe place, Z up, X and Y usually at far back and right (for an OX). If you do not have home switches, then if you turn on your GRBL controller with the machine in a safe position, critically with Z at the top of travel, then that will be the 'home' position and also the default G28 position. Or you can home/turn on anywhere you like, then SET G28 to a safe position, and then it all works as designed. However, some people are in the habit of zeroing the machine manually, then powering or resetting the GRBL controller to set 0,0,0. This avoids using 'work offsets' because, I have heard it said, they are too hard to understand. This is what will cause Gcode that uses G28 for 'go to a safe place' to fail miserably and hit the workpiece. Work offsets are simple. This is where your work 0,0,0 is. machine home is machine 0,0,0, a safe place to park. All you need to do is turn on GRBL with the machine at this safe place, with Z high up away from the work., X and Y can be anywhere though the standard is at the positive travel end. Now jog to where you want your work part 0,0,0 (which you set up in Fusion for your stock box) to be and press the 'set 0' for each axis buttons in your GUI. Now run the code. Job done. see, not hard to understand (-: Alternately you can use Stroooms nice post-processor for GRBL GitHub - Strooom/GRBL-Post-Processor: Start which does not use G28, but does rely on machine 0,0,0 being in a sensible place for safe parking.
Replying to your original post, Having just had a long discussion on Sketchup and Fusion, it seems people think it's a either or kind of thing. I luv them both. The first point I make to most people is that Sketchup is a modeling program (and very good and easy to use one at that), with CAD like ability's. Fusion 360 is a bonafide CAD program from a long established CAD company (Autodesk 1982). With Sketchup, I've actually mapped out my entire house and property here. Including the location of all underground drains, pipes, tanks, wires, etc.. Which is something you won't be doing in Fusion. At least not without massive amounts of Ram and CPU power. The other main point is that while Sketchup has always been free to use by the home user, Autodesk has never been known for it's affordable offerings. And I believe Fusion is only free to use because of Sketchup. Plus there's the intuitive and ease of use UI changes brought on by Sketchup. For instance, Trimble Sketchup owns the patent for "Push/Pull"... My main point is that climbing the steep learning curve of Fusion 360 is well worth your time, even if the Free part goes away one day. It's solid and marketable CAD skills. But your time is/was not wasted in learning Sketchup. And like me, you should always keep it on your PC...
Hi. I have been using F360 for some time as a CAD tool and continue to be mesmerised by its capabilities. I am now wanting to use it for CAM (I currently use Easel but want to progress!) does any one know of any support resources other than the Fusion 360 YouTube channel. I think I my be suffering from Lars overload(he is very good and clearly enthusiastically knowledgeable) so think I need a change of tutor. Any suggestions?
Ha! I'm currently learning Fusion 360 with Lars and my wife has suggested that I have spent more time with him recently than with her. I don't have any other suggestions but for the new user like me he is an excellent instructor.
A few more general suggestions Use this post processor: swarfer/GRBL-Post-Processor If you dont know how to use a custom post, the info is here: How to install a Personal (local) Post Processor in Fusion 360 CAM | Fusion 360 | Autodesk Knowledge Network Learn about CAM templates and how to organize your tool library. It will save you a ton of time: G Code Problems / Fusion 360 I'm no expert, but feel free to reach out if you get stuck.
