Page 1 of 3 123 LastLast
  1. Looking at adding a floating head to my new build, I've found some code that goes in sheetcam to be run before a cut, this lifts the head, drops it and zeros the DRO etc, what I can't find is where the signal from the floating head micro switch is fed into the mach3 system??

    Is it just another limit switch? Or does it need a seperate input signal?

    cant find any information on this bit.

    i guess a limit will do it as it will only close when the torch has hit metal, but wouldn't that trigger an e-stop??

  2. #2
    Post the code because chances are it uses G31 and the Probe input.? It could also need a Macro.?

    Edit: To be honest this could easily be done just by modifieing the M3 (Spindle on) macro to use G31 command and the probe input. It would then set all the Dro's etc and pierce height etc from within the Macro. All you would do is insert M3/M5 in the G-code which you may be doing anyway for torch on/off.?
    Last edited by JAZZCNC; 01-02-2014 at 02:38 AM.

  3. I have found a couple of versions, one uses g28.1 the other uses g31. The g31 version seems besta st it uses the switch connected to the mach probe input and apparently it can still allow "home all" to use the upper limit switch on the Z axis, this is exactly what I want.

    I will start on building a floating head as it seems pretty essential and makes a lot of sense to me.

    I also need to find out about editing the sheetcam post file to insert the new code.

    am I right in believing I need to use a THC post in sheetcam now instead of the basic mach3 post?

  4. #4
    To be honest I don't know enough about THC or Plasma related stuff really to confidently advise.

    If all your wanting to achive is to probe the surface then retract to a set height along with zeroing DRO's etc then that's easy enough done but you'll need to either alter an existing Macro like M3 or create your own. This macro reference you then have SheetCam insert into the code it produces at the points it's needed.

    If your wanting proper THC in that it follows a set distance from the surface then that will probably be differant matter.?

  5. I have had a look inside the post code for the mach plasma with THC option in sheetcam and it has the code for G31 seeking so it just needs some options altering and the floating head switch wired to the probe input I think.

    basically all I want is to have the torch seek the metal at the start of each cut then raise to pierce height and start.

    i also want to retain the top limit switch for the "home all" feature in mach.

  6. #6
    Quote Originally Posted by Davek0974 View Post
    I have had a look inside the post code for the mach plasma with THC option in sheetcam and it has the code for G31 seeking so it just needs some options altering and the floating head switch wired to the probe input I think.

    basically all I want is to have the torch seek the metal at the start of each cut then raise to pierce height and start.

    i also want to retain the top limit switch for the "home all" feature in mach.
    Ok that's easy enough but if you want DRO's Zeroing etc then it will need to go into a Macro file because you'll need some VB code to do it and Mach doesn't support VB directly in the G-code file.

    Regards "home all" then Mach treats homing separate and just watches the assigned pin, by that I mean it will not watch limits etc unless specificly told to do so. It will also ignore the Probe input while homing but that shouldn't be a problem.
    Also by default Mach homes each Axis individual one at a time when you press "Ref All Home" they won't all go at same time. If you want it to do this you have to alter the Homing script.
    Last edited by JAZZCNC; 01-02-2014 at 06:27 PM.

  7. The post processor I have been looking at uses g31 z -100 to drop the torch until the probe switch changes state, g92 z0.0 to zero, then g00 z25.00 to raise it by the preset distance, g92 z0.0 to zero the z axis and g00 z1.00 to preset the pierce height.

    this is from sheetcam, will that not work in mach3??

    i need to ref home one axis at a time as all my limits switches share one input pin, that's fine and works well.

  8. #8
    Quote Originally Posted by Davek0974 View Post
    The post processor I have been looking at uses g31 z -100 to drop the torch until the probe switch changes state, g92 z0.0 to zero, then g00 z25.00 to raise it by the preset distance, g92 z0.0 to zero the z axis and g00 z1.00 to preset the pierce height.

    this is from sheetcam, will that not work in mach3??
    Ok well G92 is an Offset Coordinate from the exisiting coordinate point. What it's doing is using the probe to find the material surface and where ever that coordinate falls in the current WORK Coordinate system (G54) then it sets an offset coordinate value. (g92 z0) then Moves 25 away(g0 z25) resets the offset coordinate to Zero at this point (g92 z0) then moves to 1mm above this (g0 z1).

    It doesn't actually Zero the DRO or should say Set the Zero WORK coordinate. It just applies an offset Coordinate from this WORK coordinate. If you cancel the Offset by using G92.1 you'll see the True WORK coordinate.

    Try it in MDI in simulation mode. First make sure any Offsets are cancelled by typing G92.1
    Next Zero the Work coordinates by zeroing the DRO's then jog a set distance away say 10mm positive.
    Now type G92 z0 and you'll see the Z dro change to 0 now type G0 z5 which will simulate movement 5mm positive.
    Now Cancel the Offset with G92.1.? . . . . Now you'll endup with 15mm positive in the Dro which is the true WORK coordinate. 10mm we started with plus 5mm the offset moved away from it's zero Offset coordinate.

    To be honest using coordinate offsets is not the best way to do it and can easily get you in trouble with other g-code files because they stay in affect if not cancelled. This can lead to unexpected movements and crashes.!!

  9. So it will work, but not a good method.

    is there a way to have g92.1 run at then of every cycle?

    maybe not important as every job will use the probe/offset method surely it will get set/reset many times during a job and a retained offset would only matter if I were then to run a manual part after an auto probed run??

    i gather doing a home-all would clear any offsets or not?

  10. #10
    Quote Originally Posted by Davek0974 View Post
    So it will work, but not a good method.

    is there a way to have g92.1 run at then of every cycle?

    maybe not important as every job will use the probe/offset method surely it will get set/reset many times during a job and a retained offset would only matter if I were then to run a manual part after an auto probed run??

    i gather doing a home-all would clear any offsets or not?
    Yes will work and yes there are better ways.

    No offsets are not cancelled with Ref all home this is one of the dangers with them.
    What you need to understand is there are 2 coordinate systems, WORK and MACHINE. When you Ref home you are defining the MACHINE Zero coordinate position which is fixed and never changes unless you move the Switches.
    Work coordinate Zero can be anywhere on the Machine. G92 Coordinate Offsets are offsets from currant WORK coordinate point and stay in affect until cancelled. So even if you load another G-code file the previous offsets still apply if a G92.1 hisn't given before closing the file.

    When you use G92 nothing moves it just defines a new Point which you then work from. Plus the other thing which can cause problems is that G92 only works with Absolute moves so any incremental moves will use the WORK coordinate offset.

    A much better way is to Define a user Macro which has the G31 move to find material height which then Zero's the WORK coordinate DRO's, then move to any heights you'd like. With this setup you don't run the risk of falling foul with offsets and can have much more flexabilty and control of what happens.
    You can even setup User DRO's on the screen set to enter preset and pierce height etc.
    All you do then is alter the Sheet cam post so it enters the Macro name in the G-code at the appropriate point or points needed. Mach3 does the rest.

Page 1 of 3 123 LastLast

Similar Threads

  1. NEW MEMBER: In over my head
    By Tele45 in forum New Member Introductions
    Replies: 8
    Last Post: 03-01-2014, 02:30 PM
  2. advice on floating bearing - outer ting rotating
    By dsc in forum Lead Screws, Nuts & Supports
    Replies: 8
    Last Post: 18-11-2013, 02:23 PM
  3. ballnut housing and floating end ballscrew assembly
    By dsc in forum Lead Screws, Nuts & Supports
    Replies: 12
    Last Post: 12-07-2013, 08:22 AM
  4. non-locating / floating bearing - shaft location
    By dsc in forum Linear & Rotary Motion
    Replies: 5
    Last Post: 28-06-2013, 10:07 PM
  5. Driving floating end (ballscrew)
    By blackburn mark in forum Lead Screws, Nuts & Supports
    Replies: 16
    Last Post: 11-09-2010, 11:55 AM

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
  •