489,625 active members
4,844 visitors online
Register for free
Login
489,625 active members
Page 2 of 2 12
Results 13 to 23 of 23
  1. #13
    Registered
    Join Date
    Oct 2008
    Posts
    1806
    Thank you for the video. I always like to watch good systems work. I was just making sure you understand that if you are to setup well for a consistent process that is always relative to an exact position on the machine you really need to be working with two sets of coordinates.

    One set is zeroed when you reference your machine home, and those are absolute machine coordinates.
    The second set is zeroed relative to the part when you setup a job.

    Your tool changes should be based on absolute machine coordinates.

    You can have lots more sets of coordinates than that when you start setting up different offsets if you have fixed fixtures and jigs on your machine, but that will get you started.
    Bob La Londe
    http://www.YumaBassMan.com

  2. #14
    Community Moderator ger21's Avatar
    Join Date
    Mar 2003
    Posts
    32480
    My problem or question from the beginning was how I can find that code which is embedded in the button of screenset and how the syntax should be formulated in atc macro to call z zero macro.
    If the auto zero macro is in the button, then you can't call it from the tool change macro. If you save the auto zero macro as M1111.m1s (Can be any unused M code #), then you can call it from the ATC macro with :
    Code "M1111"

    But, as I said before, I wouldn't recommend doing it that way.

    Couple questions about your macro.

    1) How are you setting Z zero? Are you placing a plate on the workpiece?

    2) How do you plan to auto zero after the tool change? What is at X100 Y 100?
    What Bob was saying above, is that it's bad practice to use:

    Code "G0 X100 Y100" ' Move to Probe position

    The reason is that this position is in the current work coordinates, and will change if you change your X and Y zero positions.

    You should be using:

    Code "G53 G0 X100 Y100" ' Move to Probe position

    Which moves to X100 Y100 in Machine coordinates. So, as long as you home the machine each time you turn it on, it will ALWAYS go to the same spot.


    If you are setting Z zero to the top of your workpiece, then running the auto zero at X100 Y100 will NOT set Z zero to the correct height unless X100 Y100 is also the top of your workpiece. You probably need to implement a fixed plate in addition to a moveable plate, and do it like I do in my 2010 Screenset or the Big Tex screenset. The difference between the two plates is stored in the screenset, and is used to set Z zero after a tool change. Watch the video to see how it works.

    Mach3 2010 Auto-Zero - YouTube

    I believe that what they are doing in the video only works because they are setting Z zero to the center of the rotary axis, so it never changes.

    Also, if you have Mach3 configured for ATC on M6, then M6End is NOT used at all. When Mach3 sees an M6, it will run M6Start, and then continue on with the g-code.
    Gerry

    UCCNC 2017 Screenset
    http://www.thecncwoodworker.com/2017.html

    Mach3 2010 Screenset
    http://www.thecncwoodworker.com/2010.html

    JointCAM - CNC Dovetails & Box Joints
    http://www.g-forcecnc.com/jointcam.html

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

  3. #15
    Registered
    Join Date
    Oct 2008
    Posts
    1806
    Not to muddy the waters, but they could have an offset programmed for the rotary axis in the OPs posted video.
    Bob La Londe
    http://www.YumaBassMan.com

  4. #16
    Community Moderator ger21's Avatar
    Join Date
    Mar 2003
    Posts
    32480
    Then it would only work for stock of a specific dimension.
    You normally can't change tools and auto zero to a fixed location unless there is some reference between the actual zero position and the position you are zeroing to.
    Gerry

    UCCNC 2017 Screenset
    http://www.thecncwoodworker.com/2017.html

    Mach3 2010 Screenset
    http://www.thecncwoodworker.com/2010.html

    JointCAM - CNC Dovetails & Box Joints
    http://www.g-forcecnc.com/jointcam.html

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

  5. #17
    Registered
    Join Date
    Oct 2008
    Posts
    1806
    I would have the offset set to center of the axis, not stock surface. You have a tool zero, and then you program the offset to the center of the axis from there. Designing parts is no harder. You just set your stock surface at the starting radius of your stock in CAM.

    I know, in ordinary 3 axis milling we usually set stock surface to zero, but we don't have to. We can use whatever is convenient for the machine setup or the part geometry.

    Anyway, I am muddying the waters and probably not helping the OP by going off on this tangent.
    Bob La Londe
    http://www.YumaBassMan.com

  6. #18
    Community Moderator ger21's Avatar
    Join Date
    Mar 2003
    Posts
    32480
    I would have the offset set to center of the axis, not stock surface. You have a tool zero, and then you program the offset to the center of the axis from there.
    What's the point of that, as they're both basically the exact same thing. Unless you want your zero plate at some other Z height.

    I know, in ordinary 3 axis milling we usually set stock surface to zero, but we don't have to. We can use whatever is convenient for the machine setup or the part geometry.
    But if you zero to a fixed location like in the Legacy video, you're Z zero MUST be the same every time, a fixed location from the plate. Or, you need to use a dual plate technique.

    My assumption is that the OP isn't using a rotary axis, but that just happens to be what the video is showing?
    Gerry

    UCCNC 2017 Screenset
    http://www.thecncwoodworker.com/2017.html

    Mach3 2010 Screenset
    http://www.thecncwoodworker.com/2010.html

    JointCAM - CNC Dovetails & Box Joints
    http://www.g-forcecnc.com/jointcam.html

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

  7. #19
    Registered
    Join Date
    Oct 2008
    Posts
    1806
    In the video he shows they are not the same thing. Atleast it does not look like it to me. The point might be that you can have preprogrammed offsets for lots of things. The corner of a vise square on the table, the center of a lathe chuck used for holding round parts, and the center of the axis of a rotary axis on the machine. You could also have your z-zero plate out of the way below the table or some other location as it appears to be in the video clip we saw.

    I've recently started playing with things like this on my big (big for me) milling machine, and its really convenient to always know exactly where the corner is of all three vises I have bolted to the table. I don't even have to go there and zero. I just refference home and select the preprogrammed offset.

    Anyway... I don't think this is really helping the OP. Not yet anyway.
    Bob La Londe
    http://www.YumaBassMan.com

  8. #20
    Registered
    Join Date
    Oct 2013
    Posts
    6
    Dear Gerry and Bob
    I really appreciate your feedback, it has helped me a lot
    My plan is actually that the machine would automatically zero absolute coordinates with the fixed mounted limit switches at start up (using a specific button ) . But it is another separate project. I am as I said before not an expert in this area and that is why I have to take it step by step.
    Bob ,,,, Immediately I assume the macro written in my previous thread is based on absolute machine coordinate. ( I'll test it for a job that involves several tool changes )
    And now I'm going back to Gerry's questions
    I have an idea to place a permanent reference plate in the same row as the tools and the code would be something like , Code " G53 G0 X80 Y20 " ' Move to Probe position (thanks Gerry )
    I thought obviously I could settle for a fixed mounted reference plate by determining workpiece height in the cam file, but I am now unsure whether this is possible ! ?
    Once again Thank you Gerry for the exciting video with many inspiring features. I will in near future download both screenset and related document to see what I can learn about it

  9. #21
    Registered
    Join Date
    Jun 2011
    Posts
    10

    Re: Mach3 ATC & Auto Tool Zero

    Hi

    i have fix the problem very easy issues working perfect.!!!!!!!!!!!!!!!!!!!!!!!!!!!!!
    do not work with the macro MACRO IS WORKING PERFECT !!!!!!!!!!!!!!

    you need to fix tool offset !!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!

  10. #22
    Registered
    Join Date
    Jan 2015
    Posts
    5

    Re: Mach3 ATC & Auto Tool Zero

    Hello i have recently made a 1.1 mtre square cnc plasma table and i have put the probe tool set up code into machine but i ave the contacts for the zero probe on a micro switch the torch head is mounted on a sprung brkt witch moves torch towards micro switch as it gently touches material tub i need the probe to raise when it hits micro switch not lower into it ie the thickness of the touch plate ..any ideas i would really appreciate any help on this matter as i know it can be done but need the info to change the code to reverse the height instead of lowering on to work minus the touch plate regards Russ Beck

Page 2 of 2 12

Similar Threads

  1. G100 + Mach3 2010 screen auto tool zero
    By Menatep in forum G-REX
    Replies: 4
    Last Post: 05-02-2014, 10:13 PM
  2. Mach3 and Auto Tool Zero / Mach Blue Probing by Big-Tex
    By TomiY in forum Machines running Mach Software
    Replies: 9
    Last Post: 11-15-2012, 09:24 PM

Tags for this Thread

Posting Permissions

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