-First, make sure you have cloud libraries enabled in your preferences. For the OpenBuilds ecosystem, we suggest using the OpenBuilds GRBLpost processor found here: OpenBuilds/OpenBuilds-Fusion360-Postprocessor To install this processor: -Click on the green "Clone or download" button. -Click on "Download ZIP" -Extract the downloaded zip file. -Open Fusion360 and open your Assets library. -Open the CAMPosts folder. -Click on Upload -Click Select -Navigate to the extracted folder and select OpenbuildsGRBL.cps -Click Upload To use this processor: -Click Post Process. -In the Post Process dialog box, click the Setup button. -Select "Use Cloud Posts". -Select "OpenbuildsGRBL" in the dropdown next to the Open config button.
I've sticky'ed it been referring to this thread far too often in support questions there days (; Thanks for the writeup @sharmstr!
Great job @sharmstr and @David the swarfer thank you for sharing this. Like @Peter Van Der Walt says this is a big one on the list of questions so having this locked down for a resource will be great. Actually now that I think about it would not hurt to have it as a proper Resource as well. If you find the time @sharmstr could you please add it to the helpful tools category of Resources. I think it really needs a spot where it will not get lost in time. Thank you in advance for your help
Don't know how forums work so if I ask a question in an inappropriate location or way, please be kind with a newby. The process to upload the file into assets above in the string worked becasue I can see it in my list of assets. However, when I try to do the setup step above to use the post process there is no option "Use Cloud Post". It is simply not in the dropdown list. It's like Fusion 360 has made a revision and this option is no longer available. I tried the other options but could not find OpenbuildsGRBL.cps to include it as a post process. I'm new to fusion 360 and to using this forum so please be patient with me. I've yet to get even one project successfully over to my Leads 1010 using Fusion 360. Thanks to anyone who will help! KaDee
Hi guys, did see @kaDee's post earlier, but been out all day. If no one else solves this for you I will have a look at my Fusion set up in the morning (getting late here in the UK). This certainly worked last time I tried it and those instructions still match what Autodesk tell you to do. Alex.
Hey guys. You need to enable cloud in your preferences. How to install a cloud post processor in Fusion 360 | Fusion 360 | Autodesk Knowledge Network
Thank You Alex. I do understand the time difference well US to UK as I speak daily on the phone to a dear friend that lives in Market Harborough, UK and I am in Arkansas, US. I really tried every available option in the dropdown box but lack sufficient knowledge to know if I'm on the right track. It is as though I have either done something wrong (which is possible since I am new to Fusion 360) or Fusion has changed the way you enable a post process not in their list of machines. I've done a few projects using Openbuilds software and normally your software meets my needs for basic signs and such but this time I could not figure out how to extrude the letters or logo to make my brass stamp I was making. At least I could not find a way to do it without 3rd party software such as Fusion 360. I appreciate you looking into it and would be delighted to have a potential success path. I will wait patiently. KaDee
Thanks Sharmstr. I enabled cloud preferences and figured out that the example they give in the link is not up to date on their website. There is no "CAM" option. Its under "Manufacture". Also, they don't tell you but you have to copy the file it into the New Post Process folder and not just into Assets directory (they don't tell you that). It then allowed me to select OpenbuildsGRBL.cps in the post process folder. Ok, so I got that figured out, I hope. But I won't know it worked until I can get it to make some tool paths and G-code. But now it keeps telling me my tool paths are out of date and won't let me save anything till I update them. And it won't let me edit them. GRRR. Every time I try, it just makes new Setups but I can't get back to the setup menus for toolpaths. It's very frustrating. And their forum is two orders of magnitude more complex to navigate than this one, especially for someone who asked their first question 3 days ago on this forum. So for now I'm stuck again. But you did answer my original question and I REALLY REALLY thank you. Openbuids team is top drawer. So how do I start a new, I think they call it a thread, to ask the question of how to clear this Fusion 360 error for out of date tool paths an get my simple block toolpaths edited and over to G-code so I can run on some program like Universal G-Code Sender or Openbuilds CAM (preferred)? Maybe that has already been answered and you can point me in the right direction. KaDee
btw, got it to work after reboot. may have been cockpit error or machine. Don't know which. But i have gcode to try! Not sure what to do with it now though whether to use gcode sender or try to load in Openbuilds CAM. I'll try both tomorrow. It did give me the same error each time I tried to generate gcode, so dont know if it will work till i try it. error when generating from F360 was "Invalid Work Coordinate System. Select WCS 1..6 in CAM software. Selecting default WCS1/G54." I will see if I can figure it out tomorrow. i. e. what it is talking about. Day too long today.... Thanks KaDee
Hi @kaDee, sounds as though you are getting there. The last question is not an error - Fusion is telling you that you didn't select a work co-ordinate system, so it is going to use the default (G54). In manufacturing (cam), setup, on the right hand side of the setup menu you can select a wcs. Until you understand how that works just choose 1 (G54) or ignore it and Fusion will choose that for you.
right click the setup select 'edit' select 'post process' set the WCS to 1 (this tells it to use WCS G54, the default system) save post the Gcode btw you may be able to right click that scroll box and select 'set as default all' which will make it the default for all future setups. as for installing the post processor, I did this last week without the cloud options. I put the .cps file in my folder where I generate all my gcode, and selected it as the post to be used. No cloud needed. That said, if you have multiple machines running Fusion and/or multiple CNC machines with different posts, putting them in the cloud for easy selection is a good idea.
Thank you gentlemen for all your help. Today, I had my first semi-successful cut (used a test board same size before I make the large brass stamp). I still had a couple of problems but I think I'm on the right track. I found that something is adding to the G-code a G53 code that sets Z-10 at the beginning and end which would have broken the 1/8" roughing bit had I not done a "bit not installed" test cut. I just commented out the g-code line and it cut the roughing pass perfectly on the board. (I've had some experience editing G-code so that is not an issue). However, the finish pass with the 1/32 bit didn't go as well. Somehow, I must have messed up in F360 and had added in some extra tool paths when I was selecting where to cut and it wiped out part of what I rough cut. So, I went back and redid the tool path and g-code for the finish pass later tonight and it looks much better on the simulation. I will run it on my machine my next day off using a scrap board before I actually cut the 1"x2"X0.250" brass block. I'd say I have a 90% chance of the cut going well and I will have produced the large branding stamp for big items with my initials. Then I will start making the smaller logo stamp for my wood turnings. It's much more difficult since it is just extruded lines, arcs and circles. Then I will put my upgrade on my LEADS 1010 high Z mod and be ready to go to the next project. Thanks again. KaDee
The post processor has options that affect these begin and end codes, you can change them and they will be remembered. So do read through the list of options . Knowledge is power! (-: Doing a G53 G0 Z0 at the begin and end of a job is an industry standard safety move. Machine home for Z is the top of travel so this moves the tool as high as possible, giving the best chance of missing all the clamps etc. But, with limit switches on GRBL if you go to Z0 it will trigger the switch, so the post allows you to enter a value (always negative) to clear the switch yet still do a safety raise. it defaults to -10 but you can change that to whatever is reliably 'enough', maybe -1 is enough on your machine. You can set these standoff values for X and Y and Z and you can turn off the goto G53 XY at the end of the job. I find I want it for big jobs so the tool clears the workpiece, but for small jobs just letting it stay at work 0,0 is fine as jogging away a little is quick.. I find that simulating a few times too many is much better than simulating too few times. check, check again, and again. I also found that making a list of steps and ticking them off as I go helps enormously. Last week I had a complicated job and the list was very useful in keeping track of what I was doing. This was a left and right wing in insulation foam, right wing has spar slot on model top, left wing has spar slot on model bottom, so the left and right sets of Gcode were different and had to be cut in the right order, aaaand when the wing is turned over the Z zero is shifted from top of material to table surface. Tool stickout was 32mm, top of material 49mm (off the table), safe travel height 54mm and Z top with that tool, 57mm. So not a lot of wiggle room. I even wrote a program to tell me the max and min Z values in a file to cross check and sure enough one of the files would have tried to retract to 67mm due to Fusions default of 10mm retract.
David that was a really good explanation. I will have to go into the post processor and see if I can set the thing to something other than Z-10. I just now realized that the G53 made it absolute machine index and not relative. That makes sense now. I'll boot up the shop laptop with Fusion 360 on it tomorrow and see if i can find the place to change it in post process instead of just changing it in G-code everytime as I have done while playing with my design. Again, very good explanation. And yes i know the value of a good procedure having been the Quality Supervisor at a Nuclear Power Plant. Thank You. KaDee
when you right click a setup or operation and select 'post process' you get a dialog, all the options you need are right there on the dialog. (reading between your lines I am thinking you are thinking you need to edit the post .cps file, but you do not need to do that since the options are on the dialog).
SUCCESS! I have created my wood projects branding stamps (Initials and Logo) in brass using my Leads 1010, Fusion 360 and the help you guys at Openbuilds have given me. I had no prior experience with Fusion 360 prior to about 2 weeks ago and had only done a few projects on my Leads 1010. Thank you for not giving up on me. I attached a photo to show it worked!
Thanks for preparing these instructions, Shawn! The Preference setting to Enable Cloud Libraries was not enabled by default on my copy of Fusion 360 version 2.0.7046 (Personal). Maybe if a check for this was inserted as the first step in the instructions it would help others who might get stuck on this (like me!) before seeing this post.
@David the swarfer (I was given your name as a good place to start). I have followed the steps in Fusion 360: grbl post processor install (the easy way) and was able to load the cps file. All seems to work well until I go through the post process steps and I get the following error. GRBL configured to mm - CAD file send Inches! - Change units in CAD/CAM software to mm. Is it possible to change a line in the cps file to have the machine default to inches instead of mm. Being in the US, we haven't caught up the the mm factor yet and although I can due the math or create a conversion chart, it would be easier to have everything default to inches.
you dont have to change your drawing (-: just select millimeters in the units field of the post, as below. the default is to send 'document units'. I don't know why the post 'requires' millimeters since I forked it and the original had that code and i did not want to mess with 2 things at once (I was focussed on fixing the arc problems) I will check later when I get a chance, got a zoom meeting just now....
Just dropped V15 which is imperial friendly. swarfer/GRBL-Post-Processor NOTE: the home offsets are still in Millimeters but will be correctly output in inches when needed. This is because Fusion does not display those numbers in the selected units, we only know the units later when processing the gcode. so by defining the number as 'always mm' we know what to do with them when inch is selected. @ClintD if you could test this carefully and let me know how it goes that would be great!
Great, it is working now by changing to mm. I have downloaded V15 and will have to load when I get a chance. Have a couple of projects that I am working on so I should have an answer later this week on how that works. Thank you for your assistance.
I have now loaded the new V15 and going through the steps to setup my machine (Workbee 1510) I am using for carving and cutting wood. I am new at Fusion 360 but seems like one of the better options for CAD/CAM and then using the Blackbox and Openbuilds control software. I understand that the CPS file should manage the post process part of the CAM and generate the correct g code. Is there a machine setup file for Fusion 360. Right now I have chosen a generic and loaded the cps file with it. I have not configured all of the setting of the generic machine. If there is a file to upload I thought that would be easier. I will follow up to let you know how the V15 appears to work. Thanks again.
Everything appears to have been created correctly and I am no longer getting an error message. Thanks for the help.
Hi and thanks for this info, I went to the CAm section of Fusion 360, I have a tool path loaded and went to the post processor tab, I saw a set up box but fount no cloud to check or uncheck? am I looking in the wrong spot?
