548,590 active members*
2,962 visitors online*
Register for free
Login
IndustryArena Forum > Other Machines > PCB milling > Autoleveler not working
Page 1 of 2 12
Results 1 to 20 of 38
  1. #1
    Registered
    Join Date
    Mar 2012
    Posts
    150

    Autoleveler not working

    I'm using the autoleveler from https://www.autoleveller.co.uk/.
    Currently I'm using the Autoleveller AE (Advanced Editor)
    I loaded the test pcb file that they have on their website and generated a probe file(gcode) from Autoleveller.

    Then I load the probe file into Mach3 and run it.
    But it just moves in a straight line in Y pauses and again moves on.
    Is doesn't do any Z movement. Although there is a G31 Z-1 command in the file.

    If I do a G31 Z-1 F100 through the MDI it does it correctly.

    I'm now on the verge of pulling my hair out.
    Is there any tutorial on how to setup Mach3 with the Autoleveller?
    Does any Safe Z setting have to be turned on or off in Mach3. Because I get messages regarding the same.

    Any help would be highly appreciated.

  2. #2
    Registered
    Join Date
    Nov 2012
    Posts
    1155

    Re: Autoleveler not working

    Please post your file(s) here, we will try to figure out what the problem is. A screenshot of Autoleveller settings would help too.

    You do not have to change anything in Mach3, but you do need to select "Mach3" in Autoleveller setup. Not sure about SafeZ, I don't think I ever changed it from the factory defaults.

  3. #3
    Registered
    Join Date
    Mar 2012
    Posts
    150

    Re: Autoleveler not working

    Quote Originally Posted by CitizenOfDreams View Post
    Please post your file(s) here, we will try to figure out what the problem is. A screenshot of Autoleveller settings would help too.

    You do not have to change anything in Mach3, but you do need to select "Mach3" in Autoleveller setup. Not sure about SafeZ, I don't think I ever changed it from the factory defaults.

    Thanks for the info, its good to hear that he problem is some minor issue.
    Files attached.

    There may be some difference in setting in the generated NC file vs the attached screen shot, since I was playing around with the settings a lot.

  4. #4
    Registered
    Join Date
    Nov 2012
    Posts
    1155

    Re: Autoleveler not working

    In the gcode you attached, Probe Depth is a bit excessive (-20mm), but that should not be a problem. It also has the Safe Height of 0, which should not be a problem either if you zero the Z axis slightly above the stock. Other than that, it looks like a perfectly working probing program (mine looks identical except for the X-Y-Z values).

    So at what point do you get the SafeZ messages? What exactly happens when you run the program? Here is the sequence you should see:
    - "Attach probe wires" message
    - move to safe height, move to bottom left corner, move to Z2
    - probe down at high speed
    - probe down at a slower speed
    - ask for the probe file name
    - move around the board and probe 80 points
    - "Detach probe wires" message.

  5. #5
    Registered
    Join Date
    Mar 2012
    Posts
    150

    Re: Autoleveler not working

    Quote Originally Posted by CitizenOfDreams View Post
    In the gcode you attached, Probe Depth is a bit excessive (-20mm), but that should not be a problem. It also has the Safe Height of 0, which should not be a problem either if you zero the Z axis slightly above the stock. Other than that, it looks like a perfectly working probing program (mine looks identical except for the X-Y-Z values).

    So at what point do you get the SafeZ messages? What exactly happens when you run the program? Here is the sequence you should see:
    - "Attach probe wires" message
    - move to safe height, move to bottom left corner, move to Z2
    - probe down at high speed
    - probe down at a slower speed
    - ask for the probe file name
    - move around the board and probe 80 points
    - "Detach probe wires" message.
    BTW. Where should I be checking for the messages?

  6. #6
    Registered
    Join Date
    Nov 2012
    Posts
    1155

    Re: Autoleveler not working

    Quote Originally Posted by ZeroBacklash View Post
    BTW. Where should I be checking for the messages?
    The messages are displayed in Mach3 status line (below the Reset button on the default Mach3 screen).

  7. #7
    Registered
    Join Date
    Mar 2012
    Posts
    150

    Re: Autoleveler not working

    Quote Originally Posted by CitizenOfDreams View Post
    The messages are displayed in Mach3 status line (below the Reset button on the default Mach3 screen).
    Ok! so I tried several things more.
    First I downloaded the older version of Autoleveler (the standard one).
    Then I generated the probe file.
    Then on running the first time it gets stuck at some point saying
    "Probe ignore activated at call for probe"

    If I rewind the code now and run it again.
    It retracts to 20mm then moves now say 5mm above the pcb.
    And then it moves and pauses only in the y axis at the pauses it should have moved in the Z direction for probing. Instead it stays at the current Z and just moves in the y direction.

    I'm trying to single step now, to find the issue however the single steppiing also doesn't work, instead the "Single BLK" LED blinks when I click the "Single BLK" button.
    " "

  8. #8
    Registered
    Join Date
    Nov 2012
    Posts
    1155

    Re: Autoleveler not working

    Quote Originally Posted by ZeroBacklash View Post
    Then on running the first time it gets stuck at some point saying
    "Probe ignore activated at call for probe"
    Is your probe working correctly? This error suggests that the probe is already touching at the moment the G31 command is called.

    Look at the Digitize signal on the Diagnostic screen. The green light should turn on when the probe is touching the stock.

  9. #9
    Registered
    Join Date
    Mar 2012
    Posts
    150

    Re: Autoleveler not working

    Quote Originally Posted by CitizenOfDreams View Post
    Is your probe working correctly? This error suggests that the probe is already touching at the moment the G31 command is called.

    Look at the Digitize signal on the Diagnostic screen. The green light should turn on when the probe is touching the stock.
    I did the and the Digitize led does light up when the probe touches.
    Also I added M0 statements after each line so that it pauses and I can debug the code. And it did do the first 10 steps correctly.
    But after the first 10 steps when I run it from there it tends to go awry. It doesn't seem to honour the G31 Z-5 step instead it just darts in a straight line.
    Could it be noise at the probe input that makes it act this way?

  10. #10
    Registered
    Join Date
    Nov 2012
    Posts
    1155

    Re: Autoleveler not working

    Quote Originally Posted by ZeroBacklash View Post
    Could it be noise at the probe input that makes it act this way?
    It is a good possibility. What does your input circuit for the probe look like?

  11. #11
    Registered
    Join Date
    Mar 2012
    Posts
    150

    Re: Autoleveler not working

    Quote Originally Posted by CitizenOfDreams View Post
    It is a good possibility. What does your input circuit for the probe look like?
    I will open the controller box and see what it looks like.
    In the meanwhile this is the controller that I'm currently using.

  12. #12
    Registered
    Join Date
    Mar 2012
    Posts
    150

    Re: Autoleveler not working

    I checked and the inputs seem to be opto isolated, so that some what minimizes the possibility of noise. I'm running out of ideas now.

  13. #13
    Registered
    Join Date
    Nov 2012
    Posts
    1155

    Re: Autoleveler not working

    It seems that some USB boards have issues with probing. Here is a thread about a similar problem:

    G31 Probe SOMETIMES works (Mach3 USB) (SOLVED) - AutoLeveller

  14. #14
    Registered
    Join Date
    Mar 2012
    Posts
    150

    Re: Autoleveler not working

    Quote Originally Posted by CitizenOfDreams View Post
    It seems that some USB boards have issues with probing. Here is a thread about a similar problem:

    G31 Probe SOMETIMES works (Mach3 USB) (SOLVED) - AutoLeveller
    Thanks for the link, the OP in that post seemed to have solved his problem with another version of Mach3. So I don't know how much it has to do with a USB controller. I have a chinese controller though.

  15. #15
    Registered
    Join Date
    Mar 2012
    Posts
    150

    [SOLVED] Re: Autoleveler not working

    Quote Originally Posted by CitizenOfDreams View Post
    It seems that some USB boards have issues with probing. Here is a thread about a similar problem:

    G31 Probe SOMETIMES works (Mach3 USB) (SOLVED) - AutoLeveller
    OK, to anyone who has this problem.
    CitizensOfDream was right it seems to be a problem related to certain USB controllers.

    So the solution is in this thread

    Aircuts on Mach3 USB NcUsbPod - AutoLeveller

    There are a number of solutions presented over there.
    By "steamer" however I directly tried the solution posted by user "Renato" where he added a dwell time before the G31 probing command

    like this

    G4 P1
    G31 Z-5 F100

    So following this I just did a find and replace of the probing lines.

    In addition I changed the probing depth from -1 to -5 as shown. so instead of G31 Z-1 F100 I used G31 Z-5 F100

    Hope this helps.

    Many thanks "CitizenOfDream" for your advice its highly appreciated.

  16. #16
    Registered
    Join Date
    Nov 2012
    Posts
    1155

    Re: Autoleveler not working

    You are welcome, glad you solved the problem.

    Instead of manually searching/replacing, you can open Autoleveller settings and change the Probe Word field to "G4 P1 G31".

  17. #17
    Registered
    Join Date
    Mar 2012
    Posts
    150

    Re: Autoleveler not working

    Quote Originally Posted by CitizenOfDreams View Post
    You are welcome, glad you solved the problem.

    Instead of manually searching/replacing, you can open Autoleveller settings and change the Probe Word field to "G4 P1 G31".
    I had tried the Custom Option settings in Autoleveller but somehow nothing was being generated in the output file. I've put in a question at the Autoleveller forum.
    Please see my post over here

    Custom options not being generated in output nc file - AutoLeveller

  18. #18
    Registered
    Join Date
    Nov 2012
    Posts
    1155

    Re: Autoleveler not working

    Quote Originally Posted by ZeroBacklash View Post
    I had tried the Custom Option settings in Autoleveller but somehow nothing was being generated in the output file.
    The file you attached there includes "G4 P1" as it should.
    As for #2002 and #500 variables, those are only used in files that combine probing and cutting. PFG files do not need them.

  19. #19
    Registered
    Join Date
    Mar 2012
    Posts
    150

    Re: Autoleveler not working

    Quote Originally Posted by CitizenOfDreams View Post
    The file you attached there includes "G4 P1" as it should.
    As for #2002 and #500 variables, those are only used in files that combine probing and cutting. PFG files do not need them.
    OK, I get it now, the #2002 and #500 are only used to store the corrected Z values into memory. so that the subsequent routing process can use these.
    Where as in PFG these are directly logged to a file and do not need to be held in memory.

    Many thanks for clearing these issues!!

  20. #20
    Registered
    Join Date
    Nov 2012
    Posts
    1155

    Re: Autoleveler not working

    Quote Originally Posted by ZeroBacklash View Post
    OK, I get it now, the #2002 and #500 are only used to store the corrected Z values into memory. so that the subsequent routing process can use these.
    Where as in PFG these are directly logged to a file and do not need to be held in memory.
    That is correct. I personally prefer using PFG and probe files. That way you can restart the program if needed (to adjust Z or to change a broken tool).

Page 1 of 2 12

Similar Threads

  1. PCB Autoleveler Plugin for UCCNC
    By cahit in forum UCCNC Control Software
    Replies: 105
    Last Post: 11-22-2019, 01:41 PM
  2. Setting drills, ID tools and back working/end working tools
    By jonathan2jones in forum CNC Swiss Screw Machines
    Replies: 5
    Last Post: 04-22-2017, 01:11 AM
  3. What is the difference between wood working and metal working routers?
    By LaughingJaguar in forum Joes CNC Model 2006
    Replies: 9
    Last Post: 10-17-2016, 07:29 PM
  4. Switch view between machine working enveloppe and job not working?
    By skillalot in forum Screen Layouts, Post Processors & Misc
    Replies: 0
    Last Post: 08-10-2015, 03:55 PM
  5. it's not working!
    By mattstiger in forum Hobby Discussion
    Replies: 1
    Last Post: 04-25-2012, 05:31 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
  •