502,702 active members
6,095 visitors online
Register for free
Login
IndustryArena Forum > CAM Software > Surfcam > path code to S post
Page 1 of 2 12
Results 1 to 12 of 22
  1. #1
    Registered
    Join Date
    Dec 2008
    Posts
    22

    path code to S post

    I'm hoping someone can help me out here...
    I am trying to get a 4 axis post working with Surfcam for our Mazak 510C.
    I have been messing around for hours trying to figure this all out and I'm stumped. I aquired two files for the S post and can't seem to get them put in the right place to work when I click on the "post" button in Surfcam. The files I have are:
    Uncx01.p2380 and Uncx01.f2380. I found several locations where there is a PostLib folder and I'm not sure which one to put them in. I messed around with this and changed the path in the PST file to:

    BeginPost 4 Axis Default:1
    PostItem MAZAK NEXUS 510
    Status Display all posts in postform.m
    ChDir "C:\SURFCAM\Velocity3\SPOST"
    Delete "%p%N.NCC"
    Command "C:\SURFCAM\Velocity3\SPOST\MPOSTWIN" "%p%n" 2380
    Task "C:\SURFCAM\Velocity3\editNC\editNC" "%p%N.ncc"
    EndPost

    I have something messed up, and can't figure it out. Could someone shed a little light on this?

    Thanks,
    Steve

  2. #2
    Registered
    Join Date
    Dec 2007
    Posts
    40

    RE: Problem path code to S post

    You have modified an Mpost PostItem instead of an Spost

    Make sure your UNCX files are in your C:\SURFCAM\Postlib\Spost folder

    Note, the INC2APT switches my not be correct for your Post

    Try this instead.

    PostItem MAZAK NEXUS 510
    Status MAZAK NEXUS 510
    Command "C:\SURFCAM\Velocity3\INC2APT" -w -5 -I "%p%n" -O "%p%N.apt"
    ChDir "C:\SURFCAM\Velocity3\SPOST"
    Delete "%p%N.NCC"
    Command "C:\SURFCAM\Velocity3\SPOST\SPOSTM" "%p%N.apt" 2380 "%p%N.ncc"
    Task "C:\SURFCAM\Velocity3\editNC\editNC" "%p%N.ncc"

  3. #3
    Registered
    Join Date
    Dec 2008
    Posts
    22

    Success!

    Darinbee...Thanks for your help! That did the trick.

    Regards,
    Steve

  4. #4
    Registered
    Join Date
    Dec 2008
    Posts
    22

    Hmmmm not quite right yet...

    Well, I can post a program now, but I'm not seeing any "A" axis moves in the program. I'm not sure if the UNCX files are any good for 4 axis milling though. I got them from Surfcam a few weeks ago. They said they were "public domain" and they may need to "contact your reseller for manipulation of this post if you need it changed". I sure would like to be able to do this myself, rather than be at the mercy of technical support. Our maintenance contract is up so we're screwed as far as help from Surfcam.

    Steve

  5. #5
    Registered
    Join Date
    Dec 2008
    Posts
    22
    Well, I messed around with this stuff all day and I have an understanding of how to modify MPosts. In the POSTFORM.M file you make your changes. As far as the Spost goes, I'm totally confused when I look at the UNCX files. It looks like there is an "s", "p", and "f" file with the same preceding number, but when you open the file, it's just an assload of numbers that don't make sense to me. I played around with the Option File Generator and was able to iron out my "A" axis positive and negative degree stuff. I don't want ANY sequence numbers in my program and I was able to get rid of all but the one at the first tool call. I also would like to be able to use G93 (inverse timing) for "A" axis work. Would anyone know how I can achieve this? Will it require a different UNCX file? Where exactly is the G93 command handled?

    Any help would be appreciated.
    Steve

  6. #6
    Registered
    Join Date
    Dec 2008
    Posts
    22
    I feel like I'm talking to myself here...LOL

    I did a little more digging and figured out where the G93 inverse timing is handled. I think I have a working post now! I still didn't figure out that sequence # problem though.

  7. #7
    Registered
    Join Date
    Jul 2007
    Posts
    148
    "SEQNO


    SEQNO/k,INCR[,m[,n]]

    k Is the starting sequence number.

    m Is the incremental value.

    n Causes sequence number output every nth block.

    This is the default condition assumed with k,m,n=1.



    SEQNO/k

    Generates a sequence number k for the next block only.



    SEQNO/0

    Causes sequence numbers to be same as .INC and CL record numbers.



    SEQNO/OFF

    Terminates sequence number output.



    SEQNO/NEXT

    Generates the next block as an alignment block with the address selected by the Configuration Tool in the sequence number.

    Related Commands:

    PLABEL/OPTION,30"

    From SPOST help menu. Maybe try using SEQNO/OFF? And yes, Surfcam forum here seems pretty dead, specially compared to Mastercam's. Which could mean that Surfcam is easypeesy to use and Mastercam is difficult or that user base of Surfcam is really small.

  8. #8
    Registered
    Join Date
    Dec 2008
    Posts
    22
    Excelmachine...Thanks a lot for the info!

    I gave my test program a shot after work tonight and I was disappointed. The tool path was real jerky...almost like it read a line stopped, then went on to the next. G9 is an "exact-stop check" and at first I thought maybe I had that in there causing this. I checked and there are no G9's. Here is a sample of my program:

    O1000
    T13 M06
    G54 G90
    S1459 M03
    G00 G43 Z3.1 H13
    X.956 Y0. A-148.355
    Z3.03
    G01 Z3. F5.
    G93
    G01 X.979 F326.087 A-143.79
    X.9951 F326.831 A-138.865
    X1.0048 F314.342 A-133.511
    X1.0083 F279.942 A-127.384
    X1.0046 F359.909 A-122.627
    X.994 F395.84 A-118.458
    X.9765 F409.97 A-114.776

    blah,blah,blah

    G94
    G00 Z3.1
    M6 T13
    G91 G28 Z0
    G28 Y0
    %

    Anyone have any ideas?

    Steve

  9. #9
    Registered
    Join Date
    Nov 2004
    Posts
    166
    Quote Originally Posted by Steve Manthey View Post
    Excelmachine...Thanks a lot for the info!

    I gave my test program a shot after work tonight and I was disappointed. The tool path was real jerky...almost like it read a line stopped, then went on to the next. G9 is an "exact-stop check" and at first I thought maybe I had that in there causing this. I checked and there are no G9's. Here is a sample of my program:

    O1000
    T13 M06
    G54 G90
    S1459 M03
    G00 G43 Z3.1 H13
    X.956 Y0. A-148.355
    Z3.03
    G01 Z3. F5.
    G93
    G01 X.979 F326.087 A-143.79
    X.9951 F326.831 A-138.865
    X1.0048 F314.342 A-133.511
    X1.0083 F279.942 A-127.384
    X1.0046 F359.909 A-122.627
    X.994 F395.84 A-118.458
    X.9765 F409.97 A-114.776

    blah,blah,blah

    G94
    G00 Z3.1
    M6 T13
    G91 G28 Z0
    G28 Y0
    %

    Anyone have any ideas?

    Steve
    Steve, I've had this problem before with Fadal machines, and it was because it wanted a G8, which made the controller "look ahead", and not do a line at a time. We were getting the jerky toolpath as you describe. I edited the post to put the G8 in, and no more problems with the Fadal. Haas machines don't seem to have this problem. It sounds like your Mazak needs the G code for this. Perhaps some one can enlighten us on which code your machine needs. Good luck.
    Hey, why's it going over there?!!

  10. #10
    Registered
    Join Date
    Jul 2007
    Posts
    148
    I agree with Cammotion, I also used to run a Fadal and G8 made the countours a lot smoother. I now run an Excel with a Fanuc 21M controller and a G8 doesn't do anything on this controller. The rest of your code doesn't ring any alarms with me, although I am more used to G54 G90 being in the same line with your X,Y and A location.

  11. #11
    Registered
    Join Date
    Dec 2008
    Posts
    22
    Thank you both for your replies. Yes, the G8 thing was the very first thing that entered my mind. I too had this experience with a Fadal. Mazak doesn't use G8. I might give it a try anyway...worse thing that can happen is it will alarm out and not work. I didn't have any time to play with this problem today, but I really need to resolve this.

    Steve

  12. #12
    Registered
    Join Date
    Jul 2007
    Posts
    148
    I'm not familiar with a Mazak but I know that some machines use custom G codes for certain things. I remember using a 4th axis on a Fadal and one of the things we did for the code was always have it spit out the code for the air brake release even if we weren't using the brake.
    I also just checked my Fanuc 21M manual and there is a code called G64. The manual states that this is the cutting mode. Some of the comments in the manual say "Once specified, this function is valid until G61,G62 or G63 is specified. The description for this code is stated as, " The tool is not decelerated at the end point of a block, but the next block is executed." G61 being exact stop mode, G62 automatic override for inner corners and G63 for tapping mode. I have never used this command in the 3 years I have been running this machine and we do a lot of 3D surfacing.
    If you can find your Mazak manual, maybe check their G code list for anything referencing inverse time or 4th axis moves? Maybe try running your post without any 4th axis moves and see if it acts the same way?

Page 1 of 2 12

Similar Threads

  1. post code trouble, or me?
    By Martin 007 in forum BobCad-Cam
    Replies: 7
    Last Post: 07-30-2008, 07:52 AM
  2. g-code path visualization ...
    By deadalvs in forum European Club House
    Replies: 4
    Last Post: 05-10-2007, 10:43 PM
  3. Gibbs post for EZ-Path lathe
    By Michael Esch in forum Post Processor Files
    Replies: 0
    Last Post: 04-10-2007, 04:41 AM
  4. Change - from linear path control to CNC path control
    By Fidibus42 in forum General CNC Machine Related Electronics
    Replies: 1
    Last Post: 12-04-2005, 05:43 PM
  5. Post Processor (ISO G-Code)
    By CNCadmin in forum Carken Products (Deskam, DeskCNC etc)
    Replies: 0
    Last Post: 01-29-2005, 02:33 PM

Posting Permissions

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