Fusion 360

New Home Forum Software Development Fusion 360

This topic contains 196 replies, has 39 voices, and was last updated by Profile photo of Saaif Saaif 2 weeks, 4 days ago.

Viewing 30 posts - 151 through 180 (of 197 total)
  • Author
    Posts
  • #22818
    Profile photo of Leo69
    Leo69
    Participant

    Rapids should only be done at a safe Z height to begin with but not a bad idea to reverse the order just in case.

    #22849
    Profile photo of vicious1
    vicious1
    Keymaster

    This is starting to become amazingly polished, Leo69 The new updates are perfect.

    Now, Not one to leave good enough alone anymore I have some more questions.

    #1

    capabilities = CAPABILITY_MILLING;
    tolerance = spatial(0.002, MM);
    highXYFeedrate = (unit == IN) ? 500 : 2100; //specify XY axis rapid feed rate in inches:mm
    highZFeedrate = (unit == IN) ? 100 : 420; //specify Z axis rapid feed rate in inches:mm

    – Can this be moved down into the User defined section to set these values in the options window for those who might want to speed it up? I tried just moving it down and that is a no go, is there a different format needed, Also can I take some of those options out somehow?

    #2 – Why is M106 getting triggered? I see ductsoup’s edit but why not use the coolant trigger or something else? Should I leave this in I guess it doesn’t hurt anything but doesn’t seem like best practice.

    #3

    N40 G1 X24.683 Y97.731 F2100
    N45 G1 Z7 F420
    N50 G1 Z2 F420

    – If we can switch the order of operations on the first 3 generated moves we can get rid of the extra z moves and use the clearance plane like intended. right now it is moving over than up, we need up then over.

    *Side note I hope this doesn’t offend any of you guys that have originally put this together That I am just jumping in here and making changes. I can move this somewhere else and fork it if you would prefer. Just let me know publicly or privately and I will move it. I don’t want to step on anyone’s toes just striving for a more perfect experience.

    #22853
    Profile photo of Leo69
    Leo69
    Participant

    Which features did you want to add/remove to user defined section? Comment out or delete the highXYFeedrate and highZFeedrate variable declarations and move them as shown below:

    //highXYFeedrate = (unit == IN) ? 500 : 2000; These can be commented out or deleted completely
    //highZFeedrate = (unit == IN) ? 100 : 400; These can be commented out or deleted completely

    // user-defined properties
    properties = {
    writeMachine: true, // write machine
    writeTools: true, // writes the tools
    preloadTool: true, // preloads next tool on tool change if any
    showSequenceNumbers: false, // show sequence numbers
    sequenceNumberStart: 10, // first sequence number
    sequenceNumberIncrement: 5, // increment for sequence numbers
    optionalStop: true, // optional stop
    separateWordsWithSpace: true, // specifies that the words should be separated with a white space
    useG0: false, // allow G0 when moving along more than one axis,
    highXYFeedrate: (unit == IN) ? 500 : 2000, // Set XY rapid feedrate – only active if useG0 is false
    highZFeedrate: (unit == IN) ? 100 : 400 // Set Z rapid feedrate – only active if useG0 is false
    };

    #22854
    Profile photo of Leo69
    Leo69
    Participant

    A couple of folks suggested putting the rapid z moves before the XY. I think I’m going to go ahead and patch the file and repost it with the Z moves first. Gimme a few minutes

    #22861
    Profile photo of Leo69
    Leo69
    Participant

    Hey guys, do me a favor and test this new post-processor when you get time. I implemented most of the suggestions in the last few posts. Also removed a hard-coded Z +10 move that was added in V5. Now that the Z moves come before the XY rapids, it wasn’t necessary anymore. The XY and Z rapids are in the user-defined section but are in MM units so keep that in mind.

    #22864
    Profile photo of vicious1
    vicious1
    Keymaster

    Soooo Close.

    There is a stray z move at the very end, and no feedrate for the last rapid move home.

    #22865
    Profile photo of vicious1
    vicious1
    Keymaster

    `G1 X181.103 Y11.18 Z-6.553 F240
    G1 X181.111 Y11.182 Z-6.483 F240
    G1 Z7 F400
    G1 Z15
    G1 X0 Y0 Z15
    M107
    M84; Turn steppers off’

    The Z7 should be the last move it is to the clearance plane. The z 15 is not needed, and the move home is not needed. The last move should just be up.
    Just to really fine tune it switch to showSequenceNumbers: false, and that beggining M106 and ending M107 shouldn’t be there (if everyone want them I can just comment them out, But I don’t really think the ramps power up an unused port is ideal). I don;t think too many have a spindle power switch.

    #22871
    Profile photo of Leo69
    Leo69
    Participant

    The Z15 and origin move at the end are hard-coded. I can go ahead and remove them. If the clearance plane is set then none of these hard-coded moves should be necessary. Easy enough to patch. I’m still scratching my head trying to figure out the mystery of the M106/M107 commands in this post. We’ll get there…

    #22872
    Profile photo of vicious1
    vicious1
    Keymaster

    The 106/7 are hard coded as well but the first is commented with ductsoup

    #22873
    Profile photo of vicious1
    vicious1
    Keymaster

    There are a few other things in there I am bot sure why they are there. I swear I saw a post generator on the fusion site but can’t find it now. Seems like there is some fluff in there I wouldn’t mind starting over. Now that I’m learning this a bit compared to arduino/c++.

    #22875
    Profile photo of Leo69
    Leo69
    Participant

    It’ll be difficult to comment out the M106 without causing syntax errors. There are a bunch of commands mapped to the fan control, not sure why. It can be removed but some people may need it. Might be better to set it up as a user-defined on/off feature.

    #22876
    Profile photo of vicious1
    vicious1
    Keymaster

    If it is a pain to chnge, I would just leave it. It doesn’t hurt anything.

    #22877
    Profile photo of Leo69
    Leo69
    Participant

    I didn’t want to change what was there so I just added a spindle option in the user-defined. Default setting is false so the M106 and M107 commands should be gone unless you need them. Sequence numbering still optional but off by default. You’ll still see the numbers in the fusion editor because the editor adds them but they won’t be there if you open in notepad or some other editor, unless you enable them of course.

    #22879
    Profile photo of Leo69
    Leo69
    Participant

    Yes, this was all new to me yesterday but very much like standard c syntax so Arduino coders will catch on fast.

    #22884
    Profile photo of Martin DB
    Martin DB
    Participant

    Sure, not so difficult if you have some minimal development skills.
    Here there are the references from autodesk:
    http://cam.autodesk.com/posts/reference/index.html

    And here a basic tutorial to code a posts processor from scratch
    https://github.com/AutodeskCAM/Documentation/raw/master/Autodesk%20Post%20Processor%20manual-sm-130829.pdf

    #22886
    Profile photo of vicious1
    vicious1
    Keymaster

    Martin – Thank you! I knew it was there. I really want to check that out. I’m going to give it a browse here in a few.

    Leo – LeoLeo Leo. You did it!!!!!

    Thank you everyone that had a hand in this from day one either Coding or testing. It looks like this is a super solid Post processor now. It behaves as you would hope/expect now. Your cuts should be much more reliable and faster with the controllable Rapids. I hope to try and put together a basics guide in the next few days to help out the experienced. Fusion is a steeper learning curve than estlcam but worth it in the end.

    Be sure to figure out what rapids work best for your machine. Don’t exceed 8mm/s on the Z and you should have no issue I will continue to use 7 on my personal machines just to be safe. If you have z axis missing step issues the highest torque is (around) 5.5mm/s and slower. (whatever 60 rpms is for your machine or less).

    So bad ass.

    Thanks again.

    #22917
    Profile photo of Martin DB
    Martin DB
    Participant

    This looks great!
    Just my two cents, I’ve merged my plasma/laser tests into V9, so now we can use laser cutter from within Fusion 360 with the same posts processor as milling.
    To enable this preview feature please see here
    https://www.vicious1.com/forum/topic/fusion-360-post-processor-for-laserplasma-cutter/

    #22919
    Profile photo of Leo69
    Leo69
    Participant

    @martin – Thanks for posting those references. I looked for a while and couldn’t find anything as useful as those. I plan to add M03/M05 spindle control to my Marlin firmware at some point and this will definitely help.

    #22943
    Profile photo of SteveC
    SteveC
    Participant

    Ryan, Leo, Martin and all,
    Sorry I missed all the fun in revamping the post file. Leo, thanks for fixing up all my hard coded hacks! I want to point out that there is one instance of hard coded positioning that remains. On tool change it moves to -20, -20, +15. This arbitrarily gave me space to insert a new tool bit. I’m not sure if there is a better way to specify this position in Fusion 360.

    I only have used this post with SD card feeding. I’m not sure if if works with Repetier Host.

    SteveC

    #22945
    Profile photo of Leo69
    Leo69
    Participant

    @stevec Most of this was just a result of the RC8 changes in Marlin. I think your hard-coded tool change move should be OK. I probably won’t be looking at this again until I add spindle PID control, but that’ll be a while. Thanks for all of your work on this too. It’s nice to have so many CAD/CAM options on the MPCNC!

    #22963
    Profile photo of Neil
    Neil
    Participant

    You all ale amazing. I have yet to touch my machine since I updated it to marlin v8 fw (and had issues). I have always wanted to use fusion to cam (I guess I will have to watch some youtube vids while I am waiting on your guide!) Keep up the amazing work all. Leo I have my laser in hand just waiting on the driver board to get in!

    I have a long weekend coming up. I have some projects to get done!

    Neil

    #22964
    Profile photo of Martin DB
    Martin DB
    Participant

    Sure Neil, just go with youtube videos for fusion, I’ve learned the basics in a couple of hours.
    Also autodesk forum is a great place to learn
    https://forums.autodesk.com/t5/fusion-360/ct-p/1234

    #22967
    Profile photo of Neil
    Neil
    Participant

    You the man Martin! thank you again!
    Neil

    #23059
    Profile photo of Bradley F
    Bradley F
    Participant

    I’ve been tinkering with fusion 360 recently to do other random things, like using the stress simulation of a 3d printable bike kickstand I designed a while back that a few people have had a few issues with, and have been staring longingly at its cam features.

    Extremely happy that we can use the cam side of fusion for mpcnc now!
    Thanks a ton!

    #24047
    Profile photo of cave
    cave
    Participant

    Wow thanks for this work guys!
    I came here looking for advice on how to get different feed rates for xy / z (I’d limited all mine to 180mm/min to avoid missed steps) and it looks like Leo has it all covered.

    Looking forward to trying out the new settings later this week.

    #24376
    Profile photo of David
    David
    Participant

    Anyone know how to get tabs to work on a Fusion 360 mesh? The only thing I’ve seen that supports tabs is 2D Contour, and it won’t let you select a face — only an outline. I can’t find a way to guide Fusion 360 to select the outline of that flat face, even though it seems to select it just fine in every other aspect of the program.

    #24410
    Profile photo of Derek P
    Derek P
    Participant

    Having big problems with Fusion 360 and wanted to see if anyone has shared my experience. I tried to generate a tool path but instead got a tooth path for an older design that wasn’t even loaded. I deleted all the cam entries and tried again. Another tool path for another older design that wasn’t loaded. Anybody seem this?

    #24456
    Profile photo of Derek P
    Derek P
    Participant

    Decided to delete Fusion 360 and re-install. Things are working now.

    #25273
    Profile photo of William L
    William L
    Participant

    Has anybody modeled the DW660 as a cutter holder in Fusion?

    #25438
    Profile photo of rkrammes
    rkrammes
    Participant

    I’m not finding this directory on my Mac. ~/Autodesk/Fusion 360 CAM/Posts

Viewing 30 posts - 151 through 180 (of 197 total)

You must be logged in to reply to this topic.