Page 1 of 2 12 LastLast
  1. #1
    I've just started to look into the g code in the programs (because I wanted to send the machine back to Z25 X0 Y0 (G0 Z25X0Y0) after the program had stopped cutting) so bear with me if I'm being a little thick. It's been 15 years since I've done any computer programming of any sort so am more than a bit rusty!!

    I'm trying to drill a few holes in my work piece (3mm lite ply) so I can put some hold down screws in to stop it from lifting (yes I know get some spiral down cutters) but I'm not sure what command to use. Basically I want to spiral drill the holes with the 2mm single flute bit I'm using and then send the spindle back to X0Y0 and wait until I've finished screwing in the screws, then when I've finished I want to be able to click the start button again and it carry on the program. I'm using CamBam but not sure if it has an option to do this?

    Can anyone help?

    Last edited by njhussey; 05-11-2015 at 07:57 PM.


  2. #2
    Hi Neil,

    Sorry I don't know what or if there is a g code command to do a pause, however you could use Feed hold in mach?, this is the same as a pause, if you wanted to you could go as far as setting up your own switches connected to inputs or if you went with OEM triggers rather than inputs you could then use hotkeys and enter the OEM numbers. So 1000 is Start, 1001 is Feed hold or you can just click the Feed hold on the Mach3 screen.

    I know this isn't really what your wanting as you want to it all to be automated, I'm just trying to help with what I can, it is a start/compromise, you could just have the machine go to Z25 X0 Y0 by adding this code to your job g code, then just pause the machine while you do the screwing down.

    I'm sure the others will be along to help you where I can't though.


  3. #3

    For a pause with resume (timed pause), you can use G4, this is a dwell and supports decimals, so for a dwell of of 120 seconds you would use the line G4 P120.


  4. #4
    JAZZCNC's Avatar
    Lives in wakefield, United Kingdom. Last Activity: 11 Hours Ago Forum Superstar, has done so much to help others, they deserve a medal. Has been a member for 6-7 years. Has a total post count of 6,171. Received thanks 1,009 times, giving thanks to others 42 times.
    Ok so lets get a bit more detail.?
    #1 Do you want to make one hole then move away and screw one screw down. Then cycle start move to next hole and repeat.?

    #2 Do you want to make all the holes then move out the way and wait for screwing down then carry on with cutting rest of the job.? Has in 2 operations with in one G-code file.?

    One is much easier than the other.! Both are relatively easy with Cam software but ones is harder than the other if hand coding but still not challenging coding so to speak if your G-code savy.

    Also do you want holes larger than the 2mm bit.? If not then just use a simple peck drilling cycle with small pecks.

    If #2 with same size hole then it's simple enough has the G83 peck drill cycle is classed has one operation even thou many holes in different locations.
    After the Peck cycle ends you send the machine to the loaction out the way then Issue a M6 tool change. This will wait for tool change and just don't change the tool and push cycle start when finished screwing down.
    Last edited by JAZZCNC; 05-11-2015 at 10:56 PM.

  5. #5
    Does Mach support M00 ? I haven't used it yet but it is just. Cycle interrupt, which waits for cycle start to carry on. Much safer than a timed pause.

    Sent from my XT1072 using Tapatalk

  6. #6
    Thanks guys, hopefully the below picture will show what I'm trying to do. There are lots of nested parts and I want to put in supporting screws to help keep the ply stable and not moving all over the place so the pieces get ruined, yes vac hold down would be nice but that's not going to happen...yet! Neither do I want to be cleaning double sided tape from the parts.

    Dean, #2 is what I want to do. I currently drill the holes (3mm from memory) using a spiral mill operation (I think!) and then want to send the spindle out the way back to X0Y0 whilst I get my cordless drill and screw in the screws. Then I want to be able to set the machine back on its merry way cutting the next operation etc. etc. till it's finished.

    Charlie, the M00 option I presume would just pause the program with the tool still over the last drilled hole?

    Lee, the feed hold runs on a bit after pressing (tried it a few times...) so not really suitable and I'm not sure I want a timed delay as I know it will either be too short or far too long....

    Click image for larger version. 

Name:	IMG_20151104_162904796.jpg 
Views:	89 
Size:	147.8 KB 
ID:	16466


  7. #7
    When I want a small pause, I add a tool-change, without really changing anything. I can then jog it away and put in screws, when I hit run again it will go to position and continue.

  8. #8
    Daft question but why aren't you edge clamping the work and running a job to put in all the hold-down screw holes in one go first, then cutting your profiles?

  9. #9
    Quote Originally Posted by sinnsvak View Post
    When I want a small pause, I add a tool-change, without really changing anything. I can then jog it away and put in screws, when I hit run again it will go to position and continue.
    What code do you put in to do that? I put in M6 and it didn't flinch, just ran straight past it?!

    Quote Originally Posted by magicniner View Post
    Daft question but why aren't you edge clamping the work and running a job to put in all the hold-down screw holes in one go first, then cutting your profiles?
    I do edge clamp it (see above pic, I use masking tape...) and do the drilling operation first...I want to know (being a complete noob) how to stop the code so I can put the screws in.


  10. #10
    As someone has said above, an M0 is the best way to pause the program.

    An example would be...
    (this is based on fanuc/has g code but the format will be the same)

    G83 Z-10 R3. Q3. G99 (drilling cycle)
    X4. Y6. (hole position 1)
    X44. Y46. (hole position 2)
    G0 Z50. (rapid away from job in z)
    X0. Y0. (rapid to home/change position)
    M0 (program stop)
    ... Continue program

    The M0 will pause the program until you press the green cycle start button again.
    Last edited by jamesgates1000; 06-11-2015 at 11:02 AM.

  11. The Following User Says Thank You to jamesgates1000 For This Useful Post:

Page 1 of 2 12 LastLast

Similar Threads

  1. Anyone got some 2.5D G-code please ?
    By dudz in forum Programmers Corner
    Replies: 5
    Last Post: 22-06-2013, 10:21 PM
  2. Cambium Code Web Tools Parametric G-code Generation
    By CambiumMachines in forum Manufacturer News
    Replies: 0
    Last Post: 09-01-2013, 03:56 AM
  3. Cnc Code Maker - 2D CAD/CAM
    By CncCodeMaker in forum Programmers Corner
    Replies: 11
    Last Post: 18-04-2010, 08:31 PM
  4. G Code help
    By moose007 in forum Programmers Corner
    Replies: 4
    Last Post: 22-05-2009, 10:39 AM


Posting Permissions

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