Please Help! I'm stuck and starting to get discouraged :( - Page 2
Close
Login to Your Account
Page 2 of 3 FirstFirst 123 LastLast
Results 21 to 40 of 52
  1. #21
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    4,249
    Post Thanks / Like
    Likes (Given)
    730
    Likes (Received)
    1784

    Default

    Have you checked your work lead for good connection? If that's no good you could be running on only the pilot arc and that would explain it turning off at prematurely.

    Sent from my SM-G973U using Tapatalk

  2. #22
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    317
    Post Thanks / Like
    Likes (Given)
    78
    Likes (Received)
    104

    Default

    Quote Originally Posted by Cole2534 View Post
    Have you checked your work lead for good connection? If that's no good you could be running on only the pilot arc and that would explain it turning off at prematurely.

    Sent from my SM-G973U using Tapatalk
    Maybe I'm wrong but it doesn't look like its turning off early, just looks like the starting is delayed....




    Adding an overlap would be a dodgy way of fixing it that would need to be adjusted whenever the feed rate was changed.

  3. #23
    Join Date
    Jul 2008
    Location
    Milverton, Ontario, Canada
    Posts
    606
    Post Thanks / Like
    Likes (Given)
    164
    Likes (Received)
    254

    Default

    Its entirely missing your lead in. Change the "N40 G4 P800." P value to 10000. , or add an optional stop after that line - if the machine will support M00

    Or, change the feedrate on line 45 to 1.0, then back to 39.37 for line 50.

  4. #24
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    4,249
    Post Thanks / Like
    Likes (Given)
    730
    Likes (Received)
    1784

    Default

    Quote Originally Posted by Hardplates View Post
    Maybe I'm wrong but it doesn't look like its turning off early, just looks like the starting is delayed....




    Adding an overlap would be a dodgy way of fixing it that would need to be adjusted whenever the feed rate was changed.
    You're right, I hadn't yet watched the video.

  5. #25
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    317
    Post Thanks / Like
    Likes (Given)
    78
    Likes (Received)
    104

    Default

    FYI it is quite bad for consumable life to run along an already cut path. It causes arc wander which leads to uneven erosion of the nozle and electrode.

    Sent from my moto g(6) using Tapatalk

  6. #26
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    4,249
    Post Thanks / Like
    Likes (Given)
    730
    Likes (Received)
    1784

    Default

    Is it possible that Mach3 is set to dwell in seconds and that the dwell value is so high that the controller disregards that line?

    Sent from my SM-G973U using Tapatalk

  7. #27
    Join Date
    Oct 2019
    Country
    UNITED STATES
    State/Province
    California
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    9
    Likes (Received)
    0

    Question

    Quote Originally Posted by Delw View Post
    It makes all the correct moves from start to finish. the problem is your plasma doesn't go on till after 2 moves.
    its right there in the video.
    so over lap the the line or turn your plasma on faster
    I can't figure out how to 'turn on the plasma faster', it is supposed to turn on as soon as I press 'Start' on Mach3, but it moves through the first few commands without turning on the torch. There must be a setting that I have wrong but for the life of me I can't seem to figure out what I am doing wrong.

  8. #28
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    317
    Post Thanks / Like
    Likes (Given)
    78
    Likes (Received)
    104

    Default

    Quote Originally Posted by Hardplates View Post
    In Mach3 you can configure it to interpret the P## as either seconds or milliseconds, I have mine set up in seconds so I would enter P0.8

    After looking at the video this is likely caused by a delay in the plasma machine itself. If you click torch on when not running a program you will likely see the same delay. The proper fix to this is to add a arc OK feedback to the controller. The workaround is to time how long this delay is and add it to the pierce time.

    I'm far from a pro but I've built a couple of industrial plasma tables from scratch in my day. 90% of my business used to be products that the first op was burning them out on the table. Mostly AR500 and 46100E
    Quote Originally Posted by newbiecnc View Post
    I can't figure out how to 'turn on the plasma faster', it is supposed to turn on as soon as I press 'Start' on Mach3, but it moves through the first few commands without turning on the torch. There must be a setting that I have wrong but for the life of me I can't seem to figure out what I am doing wrong.
    I have likely told you all you need to solve this. If you believe it is a Mach3 issue and not the plasma itself then hook a multimeter to the torch on output and see when it is sending a signal to the plasma.

  9. #29
    Join Date
    Oct 2006
    Location
    Klamath Falls, Oregon
    Posts
    3,633
    Post Thanks / Like
    Likes (Given)
    415
    Likes (Received)
    1005

    Default

    You can hear the air kick on right at the M3, then the 800ms dwell, but the arc doesn't start for another inch of travel.

    Take the torch off, and time how long it takes for the arc to start after clicking the switch.

    You need to increase the dwell from P800 to whatever will cover your arc start delay.

    From the video I'd guess the arc start delay is about 3.2 seconds.

    Your dwell should be (arc start delay + pierce time for material).

    If pierce time is 800ms for that material, you should delay for a total of 4s or 4000ms.

    If the G-code is being generated by Fusion 360, including the P800, then that's the source of your issue, not Mach, not anything else. The dwell after M3 is just too short for that plasma cutter.

  10. Likes Hardplates, newbiecnc, JDennis liked this post
  11. #30
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    317
    Post Thanks / Like
    Likes (Given)
    78
    Likes (Received)
    104

    Default

    Quote Originally Posted by Cole2534 View Post
    Is it possible that Mach3 is set to dwell in seconds and that the dwell value is so high that the controller disregards that line?

    Sent from my SM-G973U using Tapatalk
    I highly doubt that is the case as if it had no delay it should fire and begin moving before it has completed the piece, making one hell of a mess of the work and consumables. On my table I run no pierce delay at all on 1/8" and under and well under a second on 3/8" and under, but it still doesn't move before it fires. And that is with the arc ok signal on the THC I built not being read by the controller. I never interfaced the arc ok signal on this table cause I don't really need it.

  12. Likes newbiecnc liked this post
  13. #31
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    317
    Post Thanks / Like
    Likes (Given)
    78
    Likes (Received)
    104

    Default

    Quote Originally Posted by Perry Harrington View Post
    You can hear the air kick on right at the M3, then the 800ms dwell, but the arc doesn't start for another inch of travel.

    Take the torch off, and time how long it takes for the arc to start after clicking the switch.

    You need to increase the dwell from P800 to whatever will cover your arc start delay.

    From the video I'd guess the arc start delay is about 3.2 seconds.

    Your dwell should be (arc start delay + pierce time for material).

    If pierce time is 800ms for that material, you should delay for a total of 4s or 4000ms.

    If the G-code is being generated by Fusion 360, including the P800, then that's the source of your issue, not Mach, not anything else. The dwell after M3 is just too short for that plasma cutter.
    The plasma machine itself! Thank you

  14. #32
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Tennessee
    Posts
    456
    Post Thanks / Like
    Likes (Given)
    139
    Likes (Received)
    120

    Default

    first delete those z line and g92 lines. doesn't make any difference without an active z height. If you have cnc z axis then you should be piercing at 150 to 200% cutting height to save tips and improve ignition arc.
    I glanced at video, not sure if machine stopped for a second before starting cut path (not arc on, but intended cut path). 800 is really big number for dwell at that scale. 1/2 second should be fine. You have two f lines, generally your lead in is running slower, but you didn't break it down like that.
    you can check plasma start time with hand trigger to see if it fires as soon as trigger is pulled. If mach is actually throwing relay quickly is second check- which I seriously doubt if it is running on same ground as plasma machine.
    your consumables look like unshielded machine torch tips- which do things like delay plasma generation time and faulty starts... I learned this the stupid way with all error no trial. Run shielded hand torch in the hand torch.
    have small little hexagons or squares to practice on until you get the machine running, less scrap.
    If nothing else works, throw mach into the bit and byte recycling bin where it belongs and get a controller board, and a 540 which will eliminate most areas of troubleshooting.
    This machine does not have active thc or arc/pierce detection- arc and pierce is not an option for another few levels of plasmas.

  15. Likes newbiecnc liked this post
  16. #33
    Join Date
    Apr 2015
    Country
    UNITED STATES
    State/Province
    Tennessee
    Posts
    151
    Post Thanks / Like
    Likes (Given)
    100
    Likes (Received)
    24

    Default

    Delete your program and rewrite it. Check your tool settings and check your lead-in and lead-out. Most likely going to find that issue in one of those. you have a Langmuir Systems Table they have a help forum on their page with some pretty awesome guys that know these machines inside and out. This was a machine I was looking at a while back and I believe if I remember correctly there is a topic on this on that forum.

  17. Likes newbiecnc liked this post
  18. #34
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    4,511
    Post Thanks / Like
    Likes (Given)
    825
    Likes (Received)
    2444

    Default

    It's a POS homeshop "CNC" plasma and the OP is surprised it does not work like "it's supposed to"? Definitely a better topic for the zone where the OP and other hobby folks can oooh and ahhh over their rigged and hacked home builds.

  19. #35
    Join Date
    Apr 2015
    Country
    UNITED STATES
    State/Province
    Tennessee
    Posts
    151
    Post Thanks / Like
    Likes (Given)
    100
    Likes (Received)
    24

    Default

    Wow this guy what a douche it looks to me to be a CrossFire Personal CNC Plasma | Langmuir Systems

    Anyways back to topic I know with GRBL but not with Mach. I would say that M3 is the command for torch on, and it that is correct then there is your problem.
    (2D Profile2)
    N20 G0 X1.5544 Y2.1409
    N25 G31 Z-100. F39.37
    N30 G92 Z0.
    N35 M3 (Torch on right at Z0 so no pierce Height)
    N40 G4 P800.
    N45 G1 X1.5247 Y1.9463 F39.37

    So for some reason its not liking this situation try adding a Pierce Height.
    It should move from X,Y Zero, then moved down to Pierce Height (Torch Should come on during this move), pause for time determined, and lastly start cutting part design.

    Hope This Helps.

    If you need more help let me know through PM and i will get you my contact information.

  20. Likes newbiecnc liked this post
  21. #36
    Join Date
    Oct 2006
    Location
    Klamath Falls, Oregon
    Posts
    3,633
    Post Thanks / Like
    Likes (Given)
    415
    Likes (Received)
    1005

    Default

    As you noted, it's that budget plasma system, which has no Z height control. The torch is situated at a static height on the machine, so Z has nothing to do with it.

    His plasma cutter is not actually done piercing until about 4 seconds after the switch is turned on.

    He just needs to tweak the dwell at the beginning of the program, that's all.

  22. Likes lumley32 liked this post
  23. #37
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    4,511
    Post Thanks / Like
    Likes (Given)
    825
    Likes (Received)
    2444

    Default

    Quote Originally Posted by DieselMater86 View Post
    Wow this guy what a douche it looks to me to be a CrossFire Personal CNC Plasma | Langmuir Systems
    .......
    Having a link to the manufacturer does not take it out of the homeshop POS "CNC" category. The CNC zone is a much more appropriate forum for discussions about this level of equipment. Let's not lower the bar on this forum.

  24. #38
    Join Date
    May 2004
    Location
    Ridgefield, Wa USA
    Posts
    574
    Post Thanks / Like
    Likes (Given)
    192
    Likes (Received)
    70

    Default

    I would add a lead in for 2 reasons first anywhere you pierce it leaves an ugly hole and the second reason is the torch is not turning on so just add a line long enough to pierce outside the design and get the torch turned on. I would then do a lead out as well you will end up with better looking parts.

  25. #39
    Join Date
    Jul 2008
    Location
    Milverton, Ontario, Canada
    Posts
    606
    Post Thanks / Like
    Likes (Given)
    164
    Likes (Received)
    254

    Default

    There is ample lead in\lead out according to the code.
    The issue is dwell time to allow the initial pierce.

  26. #40
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Tennessee
    Posts
    456
    Post Thanks / Like
    Likes (Given)
    139
    Likes (Received)
    120

    Default

    Quote Originally Posted by Vancbiker View Post
    Having a link to the manufacturer does not take it out of the homeshop POS "CNC" category. The CNC zone is a much more appropriate forum for discussions about this level of equipment. Let's not lower the bar on this forum.
    I have not seen many post on "real" plasma setups here. What are the rules on it? must use Controlled, Fanuc, or Beckenhoff controller? Are the Chinese tables running hypertherm's industrial controller off limits (that controller should be btw)? Must be hd xpr or better plasma pack, or is simple hd good enough?


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
  •