Fusion 360 and 4th Axis Issue--STUMPED!!
Close
Login to Your Account
Results 1 to 13 of 13
  1. #1
    Join Date
    Nov 2017
    Country
    UNITED STATES
    State/Province
    Mississippi
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Question Fusion 360 and 4th Axis Issue--STUMPED!!

    We just got a new HRT160 4th axis for our Haas Mini so my experience level with 4th axis in general is pretty low. My issue is this,

    My first project for using my 4th axis is basically a cube with the same machining being done on each of the rotating sides. In F360 under Pattern, I use "circular pattern" with 4 instances. The code starts off with a facing operation, several milling operations, followed by a couple drilling operations to be repeated on all 4 sides.

    For some reason the facing and milling operations would all move to a safe Z height before the A axis rotates the part. Once the drilling cycle starts it would run correctly on the first side, then go up to the retract height but would drop back down to machine zero (tool change height) before the A axis starts rotating, which doesn't allow for enough clearance. First I tried adjusting the clearance/retract heights but this a no effect on the Z axis prior to the A axis rotating. So then I started analyzing the code and was surprised that the end of cycles between the milling operations and the drilling operations were identical. I cannot find anything in the code that would make the drilling operations return to Z zero before rotating the A xis but does not require the milling operations to do the same. I have even tried separating the drilling operations into its own program, still has the same results.

    At this point I dont know if its a F360 setting or a HAAS setting that is causing the issue.

    Thanks in advance for any help.

    Keith

  2. #2
    Join Date
    Apr 2015
    Country
    UNITED STATES
    State/Province
    Connecticut
    Posts
    214
    Post Thanks / Like
    Likes (Given)
    126
    Likes (Received)
    97

    Default

    Posting the code may help. I don’t know anything about a HAAS but you might need to cancel your canned drilling cycle prior to moving your fourth axis to move your tool to a safe height. From what you said if the cycles end the same for drilling and milling then there must be something built into your drilling cycle that screwing things up and you might have to cancel it out first.

  3. #3
    Join Date
    Apr 2013
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    720
    Post Thanks / Like
    Likes (Given)
    600
    Likes (Received)
    574

    Default

    Check your post processor - it may depend on the year of your Mini, but the max Z height probably isn't 0, it's more like -4, meaning you have 4 inches of Z travel above the toolchange height.

    Most post processors I've seen for 'Generic Haas' send Z to zero before rapids, toolchanges, etc. The problem on a Mini being that's not as high as the machine can go, which can cause weird crashes (i.e. finish a drilling cycle, go to a correct, safe retract height, then go back to Z0, putting the drill in the hole, and then moving X or Y, breaking off the drill.

    Minis have extremely limited Z as it is, which is why many folks who are going to use theirs for 4th axis work get the 'Extended Z' option, which spaces the Z axis up 4" (or maybe it's 6"?)

  4. Likes Whysosharp liked this post
  5. #4
    Join Date
    May 2014
    Location
    Los Angeles
    Posts
    350
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    65

    Default

    Hello.

    Perhaps this will help 3+2 Programming in HSMWorks Part 1 - YouTube . I think we had similar issues and fixed them with these videos. It was a while ago so I dont remember what we did but we watched this.

    EDIT
    3+2 Programming in HSMWorks Part 2 - YouTube so towards the middle of this video he talks about it. Maybe you need to select the reversal of the z axis or change the way you are paterning it. He uses seed.

  6. #5
    Join Date
    Nov 2017
    Country
    UNITED STATES
    State/Province
    Mississippi
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Thanks for the info, I will definately look into that stuff.

    Whysosharp, I tried to post the code but PM has a limit on the amount of characters in a post.

    JohnnySolidWorks, I can definately see this being the issue, thanks for the direction

    Plutoniumsalmon, Thanks as well, videos are always a good thing, I'll check them out.

  7. #6
    Join Date
    Apr 2015
    Country
    UNITED STATES
    State/Province
    Connecticut
    Posts
    214
    Post Thanks / Like
    Likes (Given)
    126
    Likes (Received)
    97

    Default

    Excellent point Johnny. two of our supermaxs have a tool change height lower than z zero similar to how the mini mill may be.

  8. #7
    Join Date
    May 2012
    Location
    Mid-Iowa, USA
    Posts
    3,551
    Post Thanks / Like
    Likes (Given)
    3448
    Likes (Received)
    2049

    Default

    You can also head over to the Fusion 360 CAM forums if you need more directed help. It supports uploading files like exported projects which can be really handy for a direct perspective of any issues you're having.

    Fusion 36 Computer Aided Machining (CAM) - Autodesk Community

  9. #8
    Join Date
    Nov 2017
    Country
    UNITED STATES
    State/Province
    Mississippi
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Not sure if I'm allowed to do this but I posted the same question on ******* before posting here which did allow me to post the code. So HERE is the link if anyone wants to check out the code.

    Sorry if posting links is not allowed.

    Keith

  10. #9
    Join Date
    May 2012
    Location
    Mid-Iowa, USA
    Posts
    3,551
    Post Thanks / Like
    Likes (Given)
    3448
    Likes (Received)
    2049

    Default

    Well from what I can see (the links are not allowed but it was easy to find) all the operations that require an A-axis movement return to G53 Z0. which is standard behavior in the generic Haas post. This can be changed, but requires a post edit.

    Again, I'd suggest hitting up the Fusion forum. Your Autodesk login should already work for the site.

  11. #10
    Join Date
    Apr 2013
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    720
    Post Thanks / Like
    Likes (Given)
    600
    Likes (Received)
    574

    Default

    Yep, looks to me like the standard end of the block added by the post processor of G53 Z0. is what's getting you. CAM knows the safe retract height for the tool relative to the workpiece but the machine Z0 is below that because of the unique Minimill Z heights.

    If you do a "find and replace" (or even just manually search and replace) those Z values, which should only be right before tool changes or A axis moves, and replace the Z0 with a safe height, you should be fine.

    Haas has a YouTube video for how to alias an M code for safe tool changes with a 4th axis in the machine which will also help with this, and prevent the next problem you're going to have with a 4th in a Mini.

  12. #11
    Join Date
    Nov 2017
    Country
    UNITED STATES
    State/Province
    Mississippi
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Atomkinder, So if I understand this correctly, since the G53 Z0 is the same for the milling runs as well as the drilling, I'm only noticing it on the drills because the bit happens to be too long to clear the fixture as the A axis turns at Z0? I'm out of the office today but will check that tomorrow morning.

    Johnny Solidworks, I thought I tried replacing them on the drilling runs and if I remember correctly the machine through an error, but I'm not positive thats what I was doing. Now that I'm alot more familiar with what is going on I'll look and try that in the morning.

  13. #12
    Join Date
    May 2012
    Location
    Mid-Iowa, USA
    Posts
    3,551
    Post Thanks / Like
    Likes (Given)
    3448
    Likes (Received)
    2049

    Default

    Quote Originally Posted by LockTech View Post
    Atomkinder, So if I understand this correctly, since the G53 Z0 is the same for the milling runs as well as the drilling, I'm only noticing it on the drills because the bit happens to be too long to clear the fixture as the A axis turns at Z0? I'm out of the office today but will check that tomorrow morning.
    Bingo.

    FWIW I have added a retract modification option to the HSM post processor before, it's not difficult. Not difficult to add a tool change position if needed also.

  14. #13
    Join Date
    Oct 2013
    Location
    New Jersey
    Posts
    743
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    621

    Default

    It amazes me how no one is bothering to learn a little G-code so they can troubleshoot a problem like this. Years ago my replacement came in the door dragging a computer loaded with MasterCam. I was programming castings from 50 year old paper drawings using parametrics so I could get the job done quickly hand coding. He didn't have a post for our machines and expected the operators to change tools by hand! Wouldn't run any programs I wrote because he couldn't read G-code to see how they worked. Heard he lasted about 3 months.


Tags for this Thread

Bookmarks

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •