Starting mid-program crash
Close
Login to Your Account
Results 1 to 13 of 13
  1. #1
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Georgia
    Posts
    7
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default Starting mid-program crash

    Is there anything to watch out for when starting a program -not- at the beginning? using G90 absolute programming..

    The actual program ran fine from start to finish but threw up a burr on the chamfer pass... I then started mid-program from the contour pass (N5640) to clean up the burr and the spindle went, or at least tried, to Z-7.ish destroying all you can imagine.

    If anyone wants to see the code....

    It's not a one off error, I ran both ways again with the same results, start from beginning and it's fine.. from N5640 and it tries to crash.
    Maybe it's just the machine, it's new but was recently updated to fix other known bugs.
    I just want to know if I'm to blame before I go pointing fingers.

  2. #2
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    North Carolina
    Posts
    256
    Post Thanks / Like
    Likes (Given)
    46
    Likes (Received)
    178

    Default

    My thought (not an expert): I don't see a G43 anywhere, which would normally be setting the tool length offset. It's possible that your control is configured to automatically set the offset at a tool call (Tn M6), but starting at the line you did skips that.

    If you insert a T33 M6 (I think the chamfer was 33) at the start of that section, is the result what you expect?

  3. #3
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    North Carolina
    Posts
    256
    Post Thanks / Like
    Likes (Given)
    46
    Likes (Received)
    178

    Default

    On second look, isn't the line you restarted from still using the face mill?

  4. #4
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Georgia
    Posts
    7
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    I'm doing tool diameter offsets in CAM, not at the control.

    It is using the same tool as the face, a 3/8 end mill. The stock is 0.097" (Y) thick so no need for a large tool.

    When I get back I'll see if adding/starting from a tool call makes the difference.
    The program always goes back to the first tool at the end of the program, it does look back and tool change to the correct tool before the crash though so maybe it won't help... hmmm...

  5. #5
    Join Date
    May 2020
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    289
    Post Thanks / Like
    Likes (Given)
    189
    Likes (Received)
    186

    Default

    Quote Originally Posted by mutiny View Post
    My thought (not an expert): I don't see a G43 anywhere, which would normally be setting the tool length offset. It's possible that your control is configured to automatically set the offset at a tool call (Tn M6), but starting at the line you did skips that.

    If you insert a T33 M6 (I think the chamfer was 33) at the start of that section, is the result what you expect?
    I agree with this^^.

    Did you hit reset before your attempted restart? If so, that may have wiped out your tool length offset.

    At N5645 Try this G43 H13 Z.6;
    The tool call up that mutiny stated would probably work as well but it might send the machine to the tool change position first. (Depends on the machine)

    Edit: You might also need to add a G54 to whatever line you're starting on. Most machines default to G54 but might be different in your case.

    Turn rapid down and single block on. Set feed pot to 0% and hit cycle start. Now turn feed pot up to allow the machine to move. If you want to stop it; turn feed pot back to zero. Watch "distance to go" screen.

    Always do this when you aren't 100% sure. It is a safe way to creep into something without crashing.

  6. #6
    Join Date
    May 2007
    Location
    Australia Qld
    Posts
    72
    Post Thanks / Like
    Likes (Given)
    18
    Likes (Received)
    34

    Default

    What machine and what control?
    none of the tool changes are using tool length comp - G43 H** , on my one machine this is fine, Siemens 828d but it has a proper restart procedure.

  7. #7
    Join Date
    Jul 2014
    Location
    Ontario, Canada
    Posts
    1,167
    Post Thanks / Like
    Likes (Given)
    768
    Likes (Received)
    752

    Default

    +1 on not calling a tool height offset. If you’re doing this on a Fanuc you’re gonna have a bad time.

  8. #8
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Georgia
    Posts
    7
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    ProtoTrak TMC7 with RMX control. I bought it as a first CNC machine to learn on...

    The conversational programming is extremely limiting and likes to break tools so I started learning CAD/CAM.

    As far as what the control requires with G code, I have no idea, there really isn't any info in the manual about it, I'm simply relying on the post within Fusion.

  9. #9
    Join Date
    Sep 2005
    Location
    Oakland, CA
    Posts
    3,153
    Post Thanks / Like
    Likes (Given)
    702
    Likes (Received)
    1042

    Default

    "As far as what the control requires with G code, I have no idea, there really isn't any info in the manual about it, I'm simply relying on the post within Fusion."

    That's like getting on a busy freeway and closing your eyes on the on ramp and hoping for the best.

    You need to spend time understanding how your control responds to program code regardless of the format. If you are running G code- the same applies- take time to understand what its telling the machine to do. You can always ask questions here when you need help, but you have to do the basic ground work.
    Lots of u-tube video out there- start with understanding what a "safe start block" is.

  10. #10
    Join Date
    Oct 2007
    Country
    SPAIN
    Posts
    6,328
    Post Thanks / Like
    Likes (Given)
    2256
    Likes (Received)
    1208

    Default

    Quote Originally Posted by Barry680 View Post
    ProtoTrak TMC7 with RMX control. I bought it as a first CNC machine to learn on...

    The conversational programming is extremely limiting and likes to break tools so I started learning CAD/CAM.

    As far as what the control requires with G code, I have no idea, there really isn't any info in the manual about it, I'm simply relying on the post within Fusion.
    I would contact SWI and ask the questions - a demo prog with a couple of toolchanges too.
    On Fanucs you'd be having cancel codes at the start of the tool to clear drill cycles etc - this may need them???

  11. #11
    Join Date
    Jul 2010
    Location
    corvallis,or
    Posts
    897
    Post Thanks / Like
    Likes (Given)
    96
    Likes (Received)
    381

    Default

    On line N0030 you call G54 to specify your work offset. When you hit reset it likely cancels the G54 which you would have to reset if you want to restart mid-program.

  12. Likes Sandoz liked this post
  13. #12
    Join Date
    Aug 2021
    Country
    FINLAND
    Posts
    1
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    0

    Default

    As mTeryk said it may be that when you skip over workpiece zero (N5465 G54), the control might use wrong zeropoint.
    You can check if this is the problem by adding another G54 over the line where you want to skip and skip to that line instead. Edit: Or note where the tool is, skip to another line after N5465,push reset and without blank and with feeds at zero of coarse try it again. You should see a ridicilous minus Z movement to come.

  14. #13
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    6,368
    Post Thanks / Like
    Likes (Given)
    5956
    Likes (Received)
    4082

    Default

    Quote Originally Posted by Barry680 View Post
    I'm doing tool diameter offsets in CAM, not at the control.
    Why on Earth would you do that?

  15. Likes mhajicek liked this post

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
  •