Welcome to Our Community

Unlock hidden features. Sign Up for Free Today!

Ggbl Panel Offsets. Trying to understand

Discussion in 'Control Software' started by Bruce Fenstermacher, May 16, 2016.

  1. Bruce Fenstermacher

    Bruce Fenstermacher Well-Known
    Builder

    Joined:
    Dec 28, 2014
    Messages:
    24
    Likes Received:
    1
    Can't figure out how to make the offset feature work. So I must not understand.

    As example I have a pen tool so work height is the table top. This is my work flow:
    1. I postion my C-Bean near the edge of the front left corner with the pen at the top of the table and I set this for zero XYZ then disconnect Grbl panel and reconnect to set all to zero. I then raise the z 1".

    I've previously created a simple 1" square box with 0 thickness in scetchup and used phlatzboyz extension to create the gcode. I've loaded this gcode in Grbl panel.

    I have 25.4 set in G55 in the x y coordinates. I have G55 as my active offset.

    What I expect to happen when I run the code is the pen to move 25.4 above and 25.4 to the right and then start running the code.

    Instead it runs the code from the x,y 0 position.

    I've attached a picute of my Grbl panel setup

    Bruce
     

    Attached Files:

  2. Bruce Fenstermacher

    Bruce Fenstermacher Well-Known
    Builder

    Joined:
    Dec 28, 2014
    Messages:
    24
    Likes Received:
    1
    Hmmm. My question has been here two weeks and no answer at all. Either I put it in the wrong place for people who might know the answer to see, no one knows the answer to my question, which I have a hard time believing, or maybe I didn't ask the question in a manner others understand.

    Let me try again. I use Sketchup to create a simple one inch square box out of some 1/8th inch light ply, I'm using a 1/16 diameter bit. I create the box in Sketchup at the inset 1/4" from the corner of the red and green pain. I use Sketchucam to create a outside tool path around the square. I have Sketchucam create the gcode.

    On my C-Beam I move the bit to the left from corner 1/8" above the waste board. I set this position as o, o, o. If I start the gcode I created earlier from this point the bit will move, allowing for bit diameter, 7/32 up and right and start the cut.

    I want to tell Grbl Panel to move 2" right and 2" up from o, o, o, and start the cut. I can go back to my original drawing in Sketchup and move the box that distance and then regenerate the gcode but that is a lot of trouble.

    How do I use the offset function of Grbl Panel to do this? How would I use it to cut two boxes next to each other with an offset? I think the software can do that.

    Thanks

    Bruce
     
  3. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    521
    Likes Received:
    250
    I left this as I thought it was a repeat of a question I was already answering, sorry.
    Those answers are here and explain the difference between machine coordinates and work coordinates.
    Confused about homing, machine position, zeroing, etc

    What you are trying to do is set the machine co-ordinates for co-ordinate system G55.
    You can do this in 2 ways:
    first
    give the manual command G55 to set that active
    now jog the pen to the position you want.
    click the '0' button next to X and Y co-ordinates (or the 'set XYZ zero' button on the Work page).
    This saves the offsets for G55 so that when G55 is active, 0,0 will be where you put the pen.

    You can do the same thing for G54 through G59 and have 6 offsets so that you can select each offset in turn and run Gcode there, and have 6 identical items cut out for you in different places. You can even edit your Gcode file to have
    G54
    cut code copy 1
    G55
    cut code copy 2
    G56
    cut code copy 3
    etc
    to automatically cut the same shape up to 6 times.

    second way is to go to the 'offsets' panel
    type the offset you want into the box you need, say the X box next to G55
    now double click the box to save the setting.
    you need to do this for X and for Y separately.

    SO if I have the tool at near,left of the cut area, and start GRBL, every value in the offsets table is 0, machine position is 0,0,0 as well.
    (do not move the tool at this point)
    now I type 25 in the G55 X box and double click, then the same for Y
    then click 'retrieve' button, I should see 25.00 in the X and Y boxes next to G55

    now if I go back to the 'work' panel and issue 'g55' manual command to activate the G55 co-ordinates, I will see the work offsets change to -25 for both X and Y. The tool does not move!
    Now the command 'G0 x0 y0' will move the tool 25mm right and away to the G55 0,0 position, so if you started your Gcode file now, the cut would be at that defined 0,0 position.

    make sense?
     
    Joe Santarsiero likes this.
  4. Joe Santarsiero

    Joe Santarsiero OB addict
    Staff Member Moderator Builder

    Joined:
    Oct 30, 2014
    Messages:
    647
    Likes Received:
    134
    Did we discuss modal/non-modal in that other thread? I don't think we did :)
     
  5. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    521
    Likes Received:
    250
    good question Joe!

    In Gcode, some commands are modal, that is, they stay set until changed.
    For example
    M03
    turns on the spindle in clockwise direction, and the spindle stays on until
    M05
    turns it off.

    G01 is also modal though most Gcode does not use it as such
    G01 X5 Y7
    X7 Y10
    does the same thing as
    G01 X5 Y7
    G01 X7 Y10

    In the same way the co-ordinate systems are modal, once active they stay active until changed (and possibly even through power resets, depending on how much state information the controller saves).

    So, GRBL starts with G54 active and you need never change it if you don't use multiple fixtures etc.
    But if you issue a
    G55
    command, that system will stay active until changed, and so on.

    A co-ordinate system that IS NOT MODAL is the machine co-ordinate system. To use it you have to specify G53 on every line:
    G53 G0 X0 Y0 Z0
    will position the tool to the machine home (where it might access the tool changer)
    G53 G0 Z-20
    might then pick up the new tool, but the point is that G53 has to be on every line that wants to use machine co-ordinates in this way.
     
    Joe Santarsiero likes this.
  6. Joe Santarsiero

    Joe Santarsiero OB addict
    Staff Member Moderator Builder

    Joined:
    Oct 30, 2014
    Messages:
    647
    Likes Received:
    134
    How about F and S commands Dave. Are these modal too?:rolleyes:
     
  7. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    521
    Likes Received:
    250
    Yeah, F and S (Feedrate and Spindle speed) are modal, if you do
    M03 S1000
    M05
    M03
    the spindle comes back on at 1000rpm, same with feedrate, once you set it it will stay set.
    This means you need to have both spindle speed and feedrate set at least once at the top of every Gcode file so that you get know values. Picture this, you have just run a cut in balsa wood at 300inches a minute at 30000rpm and then change to aluminum. Bit of a shocker when the machine starts ripping though the ali (till the bit breaks) when it should be doing more like 20000rpm at 50IPM (-:

    Many others too, G81 hole drilling etc.
    Read all about it at (the unofficial/official reference)
    http://linuxcnc.org/docs/html/gcode/g-code.html

    (but do note that GRBL and other microcontroller based systems do not support all the codes listed there, if you need them then look at using LinuxCNC or Mach3), but the reality is that using just the basics that GRBL supports, you can do everything those advanced commands can do.
     
  8. Joe Santarsiero

    Joe Santarsiero OB addict
    Staff Member Moderator Builder

    Joined:
    Oct 30, 2014
    Messages:
    647
    Likes Received:
    134
    I truly was thinking about S too. Added to post.

    Personally, I have a bad habit of proofing a job partial way through, hitting estop, sending a G28, hitting cycle start. Guess where it goes? Right to the next line and at my G0 feedrate(from the G28).
    At least I still have the habit of keeping my paw on the Estop. It doesn't always save the part, but it usually saves the tool....well..most of the time!
    I put a post-it on my laptop reminding me to rewind. Seems to help.
     
  9. Bruce Fenstermacher

    Bruce Fenstermacher Well-Known
    Builder

    Joined:
    Dec 28, 2014
    Messages:
    24
    Likes Received:
    1
    David, thank you. I did find the other thread but got lost trying to use and make sense of it. This explanation makes sense to me. One thing I keep forgetting using Grbl Panel is to double click for something to be saved. I find this cumbersome specially when trying to change the basic setup. But that is another story. I did try to learn what was said at the other thread and apply it and see how it worked and learn from it but the darn double click I forgot didn't allow me to be successful.

    I also and not at the point I know gcode to understand what I'm trying to do. I haven't tried editing gcode or even sending a manual code. After all what code would I send. About the only manual thing I do at this point is jog the machine around and I've learned how to set 0, 0, 0. I've run some gcode created with SketchUcam but just couldn't figure out exactly how to plane where the gcode would cut.

    Thanks again

    Bruce
     
  10. GerritV

    GerritV Journeyman
    Builder

    Joined:
    Jul 22, 2015
    Messages:
    44
    Likes Received:
    8
    I will see what I can do about the double-click thing. I vaguely recall having trouble using something else for that but that was then. I know that with my arthritis getting slowly worse that double-clicking is becoming more of a challenge on bad days :)
     
  11. Bruce Fenstermacher

    Bruce Fenstermacher Well-Known
    Builder

    Joined:
    Dec 28, 2014
    Messages:
    24
    Likes Received:
    1
    GerrvitV,

    Thanks for considering a change to the double clicking thing. I've operated a lot of software over the last 30 years and have never run across double clicking to save something. I don't know how others feel but I dread changing a setting because I just haven't warmed up to exactly how to successfully do it. Maybe it's not the double clicking but the communication timing with the controller board. It took me a frustrating 2 hours to successfully change the initial setup.

    Bruce
     

Share This Page

  • About Us

    The OpenBuilds Team is dedicated helping you to Dream it - Build it - Share it! Collaborate on our forums and be sure to visit the Part Store for all your Building needs!
  • Like us on Facebook

  • Support Open Source FairShare Program!

    OpenBuilds FairShare Give Back Program provide resources to Open Source projects, developers and schools around the world. Invest in your future by helping others develop theirs!

    Donate to FairShare!