540,538 active members*
5,464 visitors online*
Register for free
Login
IndustryArena Forum > MetalWorking Machines > Milltronics > Partner 1 Drilling issues with Fusion
Results 1 to 6 of 6
  1. #1
    Registered
    Join Date
    Feb 2016
    Posts
    3

    Partner 1 Drilling issues with Fusion

    Have an older (1994) Milltronics Partner 1. Any time I do a drilling cycle (drilling, tapping, deep drilling etc) with multiple holes of the same diameter I have to manually edit the post so that each hole coordinate has the appropriate gcode in front of it. If I do not it will drill the first hole and then rapid over without retracting to the next location, breaking the tool.

    Here is an example of what the current post outputs on a simple 4 hole example.
    ...
    N11 G98 G81 X-0.85 Y0.6 Z-0.54 R0.16 F22.9
    N12 X0.05
    N13 Y-0.5
    N14 X-0.85
    N15 G80


    That needs to be manually changed to this

    N11 G98 G81 X-0.85 Y0.6 Z-0.54 R0.16 F22.9
    N12 G81 X0.05
    N13 G81 Y-0.5
    N14 G81 X-0.85
    N15 G80


    While not too much of an issue I have a job with 700 holes coming up and I don't want to have to manually enter that for all of them. Does anyone know if this is an issue/setting on the machine or the Fusion Post that is to blame?

  2. #2

    Join Date
    Mar 2019
    Posts
    28

    Re: Partner 1 Drilling issues with Fusion

    When I get home this afternoon I can send you my post that I've been using for a couple years now that works well with my 96 partner 1 and f360.

    Sent from my SM-N960U using Tapatalk

  3. #3

    Join Date
    Mar 2019
    Posts
    28

    Re: Partner 1 Drilling issues with Fusion

    Also g98 is initial level return, g99 would go back to your R plane. May also have to do with your height settings in fusion for your drilling operation.

    Sent from my SM-N960U using Tapatalk

  4. #4
    Registered
    Join Date
    Feb 2016
    Posts
    3

    Re: Partner 1 Drilling issues with Fusion

    Contact Milltronics about it and they said it should be

    N11 G98 G81 Z-0.54 R0.16 F22.9
    N12 X-0.85 Y0.6
    N13 G81 X0.05
    N14 G81 Y-0.5
    N15 G81 X-0.85
    N16 G80

  5. #5
    Registered
    Join Date
    Sep 2010
    Posts
    493

    Re: Partner 1 Drilling issues with Fusion

    G81 is modal, you need to move to the XY position before you call it up, you need the same XY position in the G81 line, but after that, you do not need G81 called out in every line. I also do G99 on the G81 call line, that way it stays at whatever R level you call for between moves, and then put the G98 on the last position line, followed by G80 to cancel the canned cycle.

    This methodology is the same for all canned cycle calls too, G73, G83, whatever...

  6. #6

    Join Date
    Mar 2019
    Posts
    28

    Re: Partner 1 Drilling issues with Fusion

    Here is a sample of code from a drilling cycle from one of my programs using my post for F360. Works well for me. I also attached my post processor that you're welcome to try. The usual applies - use at your own risk, etc. You will have to change the file extension back to .cps and you should be able to use it for fusion.

    (DRILL1)
    M1
    T4 M6
    S8500 M3
    G54
    G0 X0.58 Y-1.7
    G43 Z0.09 H4
    M8
    G98 G81 X0.58 Y-1.7 Z-0.515 R0.09 F30
    Y-0.3
    X2.58
    Y-1.7
    G80
    G0 Z0.09
    M9
    M5
    G32

Similar Threads

  1. Partner 6 Z-axis Issues
    By HawkinsTech in forum Milltronics
    Replies: 3
    Last Post: 07-16-2018, 06:06 PM
  2. Replies: 1
    Last Post: 10-05-2017, 03:35 PM
  3. Homing issues on Partner 4
    By Brian L in forum Milltronics
    Replies: 7
    Last Post: 03-01-2013, 10:42 PM
  4. Partner 1 rigid tapping issues
    By jswalwell in forum Milltronics
    Replies: 1
    Last Post: 04-28-2009, 02:12 PM
  5. Partner VM17 issues
    By br1 in forum Milltronics
    Replies: 4
    Last Post: 11-14-2007, 03:57 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
  •