524,117 active members*
2,068 visitors online*
Register for free
Login
IndustryArena Forum > CAM Software > SolidCAM for SolidWorks and SolidCAM for Inventor > 4 Axis Mach 3 Postprocessor (free but kinda wip)
Page 1 of 5 123
Results 1 to 20 of 97
  1. #1
    Registered
    Join Date
    Jul 2012
    Posts
    38

    4 Axis Mach 3 Postprocessor (free but kinda wip)

    I've got a postprocessor working on my homebuilt cnc mill running Mach3, which works with SC2014, tested both for wrap functions and sim5x.

    This hasn't been done by anyone who really knows what they are doing, so if you wish to use it, be aware it might not perform as expected. As such, I'm including my machine simulation data as well so we can do some collaborative efforts from here

    One of the things I'm not sure I got right is the trig translation of Y and Z around the rotary axis within the post file; I get the feeling this should not have to be done there, but it does work...

    Attachment 263678

    I used this video to learn how to set up the machine sim https://www.youtube.com/watch?v=OXmKXG8l1xA and by comparing with other postprocessors and machine defs I cobbled together a solution.

    Think I'll get email notifications on this thread so will help others as I get time...

  2. #2
    Registered
    Join Date
    May 2014
    Posts
    3

    Re: 4 Axis Mach 3 Postprocessor (free but kinda wip)

    Hello Bogan, thanks for the files Gpptool. I try it in Solidcam 2014 and Mach3.
    I put all the files in the respective directory and it works at %50.
    I would like to make same that you for my home built CNC. How do you make postprocessor and how i can watch the youtub video ? It say the video is private.

    Thanks

  3. #3
    Registered
    Join Date
    Jul 2012
    Posts
    38

    Re: 4 Axis Mach 3 Postprocessor (free but kinda wip)

    It says the same thing for me now, not sure what is up with that as it was a really good resource.

  4. #4
    Registered
    Join Date
    May 2014
    Posts
    3

    Re: 4 Axis Mach 3 Postprocessor (free but kinda wip)

    Hi, thanks for reply. i try to understand how it work and maybe later i found the solution.

  5. #5
    Registered
    Join Date
    Jul 2012
    Posts
    38

    Re: 4 Axis Mach 3 Postprocessor (free but kinda wip)

    yeh, I guess the best way would be to start with something that works, and modify the files as required to end up with your machine.

    A tip though, the .vmid files must have the same axis topology and definitions in them that the machsim xml file does. I also found adding axes to the vmid files was quite buggy, and ended up using an existing one which was compatible with my machine style.

  6. #6
    Registered
    Join Date
    May 2014
    Posts
    3

    Re: 4 Axis Mach 3 Postprocessor (free but kinda wip)

    I found this somes files and i tested Fanuc_2013 and Fanuc_2013_4X, they works with mach3 at 3 and 4 axis (good).
    But i don't understand VMID and if it is necessary to have the XML file ?
    I see your FOLDER with stl and xml files, how do you make your own machine with the STL files ?
    Thanks

  7. #7
    Registered
    Join Date
    Jul 2012
    Posts
    38

    Re: 4 Axis Mach 3 Postprocessor (free but kinda wip)

    There is a little program in the solidworks program files called MachineIdEditor.exe which you use to make the xml file for your machine definition; and add the stl files as 'geometry' to that in the correct layout. You should be able to open my (and others) xml file with that and get a bit of an idea what yours needs to look like.

  8. #8
    Registered
    Join Date
    Dec 2014
    Posts
    14

    Re: 4 Axis Mach 3 Postprocessor (free but kinda wip)

    Being complete noob to whole cnc now struggling with g-code to Mach3 issues. I just started to use SolidWorks and now testing SolidCam2014. However I cannot get out gcode which works out-of-the-box, file always contains something which mach3 does not understand or support. Yesterday I tested maitresyodas Fanuc_2013 files and managed to get almost working gcode...there was (if remember correctly) code "M05.1 Q1 or Q0 which prevented program to run. Removing those lines file was working almost 100%. My machine is chinese "6040", 1500GT-USB-3-axis to be exact.

    Any advises how make things to work easy way and not always clean manually cgode files? Is the solidcam overkill for 6040 or is there some obvious what I´m missing?

  9. #9
    Registered
    Join Date
    Jul 2012
    Posts
    38

    Re: 4 Axis Mach 3 Postprocessor (free but kinda wip)

    Have you tried this postprocessor (it'll do 3 axis no worries)? It is based on a mach3 one which works with no cleaning required for me so it should do the same for you...

  10. #10
    Registered
    Join Date
    Dec 2014
    Posts
    14

    Re: 4 Axis Mach 3 Postprocessor (free but kinda wip)

    You mean your "JohnMill" etc files above? No I havent, just Maitresyoda´s version. It´s kind of PITA to find working solution as everybody claims that they have working post for mach3....But I´ll try your files today.

  11. #11
    Registered
    Join Date
    Dec 2014
    Posts
    14

    Re: 4 Axis Mach 3 Postprocessor (free but kinda wip)

    Just dropped bogan´s files into cam and run comparison g-codes. At 1st look it seems that G5.1 Q1 is not there so it might work. However I do not like G53 as without homing switches (proximity sensors are on their way...) and being lazy/un-experienced my machine coordinates can be just anything...

    For comparison:
    Fanuc_2013:

    %
    O1
    G21
    G17 G40 G49 G80 G90
    G91 G28 Z0 M05
    M09
    G49
    G5.1 Q1
    T3 M6()
    T3
    G90 G00 G54 S10000 M3
    G0 X30.908 Y-16.689
    G43 H3 Z5. M8
    G0 X30.908 Y-16.689 Z5.
    X30.908 Y-16.689 Z5.
    Z-1.061
    G1 Z-3.061 F150
    X31.048 Y-16.679 Z-2.926 F1000

    And JohnMill:

    %
    O1 (TIKKAMODULITUKKI1_MILLING)
    N5 G0 G40 G49 G80 G21 (Initialisation)
    N10 G0 G53 Z0 (Go To Machine Origin)
    N15 G0 G53 X0 Y0
    N20 (Outil n° 3 - Diametre 3.0 D3 H3)
    N25 T3 M6 D3 H3
    N30 S10000 M4
    N35 M8
    N40 (HSS-PC-H-faces8)
    N45 G0 G54 X30.908 Y-16.689
    N50 G43 H3 Z5.
    N55 G0 Z-1.061 A0.
    N60 G1 Z-3.061 F150
    N65 G1 X31.048 Y-16.679 Z-2.926 F1000

    EDIT: Made test run and otherwise JohnMill works perfectly, last few lines get looping:

    N17955 G0 Z-0.81 A0.
    N17960 G0 Z5. A0.
    N17965 G0 G53 Z0 M9 (jumps from here back to N17960)
    N17970 G0 G53 X0 Y0 M5
    M30
    %

    EDIT2: Made dry run with file which contains roughing, 3D surfacing + 3x drill operations. It seems that there is now break for tool change (not a big deal) but main concern was drill operation which was stuck in first hole...never ending drill with same position...

    N99000 (D-drill2)
    N99005 G0 G54 X38.184 Y-9.275
    N99010 G43 H7 Z5.
    N99015 G83 Z-15.005 R-0.5 Q3. P0 F150 (kept drilling this position)
    N99020 X50.184
    N99025 X62.184
    N99030 G80
    N99035 G0 G53 Z0 M9
    N99040 G0 G53 X0 Y0 M5
    M30
    %

    Any ideas how to proceed?

  12. #12
    Registered
    Join Date
    Aug 2013
    Posts
    188

    Re: 4 Axis Mach 3 Postprocessor (free but kinda wip)

    well, finally soneone with the skills went on this road. I have my little machine with the 4th axis (i can assemble it either for rotate over X or over Y). from what I'v seen the fanuc_2013_4x is a machine that the table rotate over Z right?

    from my understanding (after opening your macsim with the machineIDEditor) you added a C subaxis of A on the rotary section to rotate over X, so my guess you did change/created the post processor to work with the C instead of the A am I right? I'm new on this post processor stuff and I'll be needing a 4th axis rotating over X or Y (it really doesn't matter each one because I can assemble the 4th axis whatever I want so).
    I know somthing about programming and having some examples to follow/understand what each command do/need to do I can provide help! I'm with the solidcam 2013 so I couldn't try your post processor (It won't appear on my processor list) but I'm about to try the SC2014 and see what have you done!

    best regards

  13. #13
    Registered
    Join Date
    Jul 2012
    Posts
    38

    Re: 4 Axis Mach 3 Postprocessor (free but kinda wip)

    The A axis is the one used (rotates around X), C is left in there as a dummy axis so I can use the 5 axis operation (you can lock C or otherwise render it unused).
    I think in 2014 they changed the postprocessor files, now the preprosseor is included in the vmid or something... Let me know how you get on with it.

    I had a go doing some indexial 4th axis work the other day, but I couldn't figure out how to set the A axis to rotate 90 between operations so a profile could be done perpendicular to a pocket... New to the 4th axis thing so not sure if it means setting up new coord systems etc.

  14. #14
    Registered
    Join Date
    Aug 2013
    Posts
    188

    Re: 4 Axis Mach 3 Postprocessor (free but kinda wip)

    well I'd already instaled the SC2014 and now I can see the johnmill machine. now I have a question, when I create the cam part do I have to go some where to enable the 4th axis?

    I'm new to this 4th axis stuff, I'd seen some videos and the guy explaining always had to enable the 4th axis somewhere in the machine options when creating the SC part.

    edit:
    well, I'd been messing arround with this and I managed to create the gcode for my part, It's a very simple part but I felt an huge victory! XD
    but I'm not able to simulate your machine it says that the machine cannot be found but I have the folder Johnmill on the proper location... I guss I'm missing something...

    best regards

  15. #15
    Registered
    Join Date
    Jul 2012
    Posts
    38

    Re: 4 Axis Mach 3 Postprocessor (free but kinda wip)

    Have you put the xml and step files in the machine location as well as the files in the postprocessor directory? you might need to change the cam part definition and set the machine file to those as well.

    Hard to tell what you're missing as I've not done an install from scratch as I was developing all the files as I went...

  16. #16
    Registered
    Join Date
    Aug 2013
    Posts
    188

    Re: 4 Axis Mach 3 Postprocessor (free but kinda wip)

    hi, yes I placed the JohnMill (with the sTL files) folder in the tables/machineSim folder and the post processor in the gpp folder...

    edit: well i think I have to place the JohnMill folder in tables/machSim/xml folder... gonna try it now

  17. #17
    Registered
    Join Date
    Aug 2013
    Posts
    188

    Re: 4 Axis Mach 3 Postprocessor (free but kinda wip)

    well I thought I'd successfully made my piece but it happens that the A axis is not rotating, on simulation moe it works great but the output gcode always reffer to A at 0, all lines including the A axis have A0. so no rotation I have to take a closer look at it... I'll try the fanuc that matresyoda posted and see if it outputs the gcode ok.

    I'll keep you posted

    BTW. about the machine sim I'd placed the JohnMill folder on the machSim and on machSim/xml and now it works nice!

  18. #18
    Registered
    Join Date
    Aug 2013
    Posts
    188

    Re: 4 Axis Mach 3 Postprocessor (free but kinda wip)

    Today I tried the fanuc, first I'd to change the rotation axis, by default it rotates over Z and that's no right for me. I've made 2 backups and changed one for rotation over X and other for rotatiion over Y so I can mount my 4th axis how I need.

    it worked very well, I've only made some index rotation (I think that's what you call it, id machines one side, then rotate then machines that side and so on) but on this test it worked flawless!

    I have to try some more deep machining but so far so good.

  19. #19
    Registered
    Join Date
    Jul 2012
    Posts
    38

    Re: 4 Axis Mach 3 Postprocessor (free but kinda wip)

    Good to hear, so is this the fanuc machine definition running with the postprocessor I made, or is it all fanuc?

    How did you get it to do index rotation in solidcam?

  20. #20
    Registered
    Join Date
    Aug 2013
    Posts
    188

    Re: 4 Axis Mach 3 Postprocessor (free but kinda wip)

    it's all fanuc, the only change I made was the retational axis. By default it came with the table rotating over Z and I changed to rotate over X.

    in solid cam what I did was:
    1 - made the milling operation on the first face
    2 - used the Transform function on that operation (right click the operation, click transform), a window will appear, select the operation on that window and after that click the button 4th axis.
    3 - now a new window will appear and you can you insert the rotations you want. in my case I needed the perform the same operation in 3 "equal sides" of a cylinder so I checked the box "include initial position" and it add the angle "0º", then I inserted 2 steps of 120º and it adds the 120º and 240º and it will perform the same operation at 0º, 120º and 240º.
    like I said it was a very simple part but it's my very first use of the automated 4th axis.

    attached I leave the post processors that I changed. I'll tell again, they are the exact same as the originals but the rotational axis is over the X or Y (fanuc_2013_4X_custom rotates over X and the fanuc_2013_4Y_custom rotates over Y)

Page 1 of 5 123

Similar Threads

  1. Postprocessor Camworks to Mach 3
    By mazaracing in forum CamWorks
    Replies: 1
    Last Post: 02-11-2011, 10:29 PM
  2. 5th axis kinda
    By Delw in forum Haas Mills
    Replies: 4
    Last Post: 12-14-2010, 03:37 PM
  3. Mach 3 Postprocessor for SolidCam
    By Debos in forum Screen Layouts, Post Processors & Misc
    Replies: 3
    Last Post: 06-20-2008, 11:15 PM
  4. 2UVR x-axis powerfeed sorta kinda working
    By Stinson_Voyager in forum Tree
    Replies: 4
    Last Post: 01-14-2007, 08:11 PM
  5. 2UVR x-axis powerfeed sorta kinda working
    By Stinson_Voyager in forum Tree
    Replies: 0
    Last Post: 12-27-2006, 06:10 PM

Tags for this Thread

Posting Permissions

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