515,089 active members
4,806 visitors online
Register for free
Login
IndustryArena Forum > GENERAL MANUFACTURING PROCESSES > TURNING > HMC Program Trouble with G03
Results 1 to 1 of 1
  1. #1
    Member
    Join Date
    Jul 2019
    Posts
    1

    Exclamation HMC Program Trouble with G03

    Im having trouble with the arc motion on a G03 move. I have a feeling the machine doesn't think the geometry matches up within .001, but I have double and triple checked my math. I have also played around with the values of x and z to see if I can find the difference in logic between me and the machine, but it must be greater than .001 because I incremented x and z by .0001 ten times both positive and negatively and simulated it each time and go the same error.
    Here is the program;
    %
    O51712(PRESSURE BLOCK)
    (MATERIAL -YELLOW BRONZE)
    (ORIGIN-X,Y,Z ORIGIN CENTER OF STOCK RADIUS MINUS .150 CLEANUP)
    (TOOLS)
    (TOOL - .200 SQUARE GROOVE TOOL)
    (TOOL -55 DEG)
    G18 G20 G40 G80 G90 G99
    G00 G28
    (55 DEG-FACE AND TURN)
    T101
    G50 S150
    G96 S60 M03
    G00 X18.5
    Z1.0
    G01 Z.250 F.05 M08
    G71 P001 Q002 D.05 U.05 W.05 F.005
    N001 G01 X0.0 Z0.0
    N101 G03 X16.5 Z-.943 K-42.0
    N102 G01 X16.5 Z-1.125
    N103 G02 X16.75 Z-1.125 I .125
    N104 G01 X17.00 Z-1.125
    N002 G01 X17.0 Z-3.0
    G01 X18. Z-2.0 F.05
    M05
    M09
    G00 G28
    M00
    ;;
    The error occors on N101, but only when it takes the finishing pass of the G71 canned cycle.
    So the simulation will run through the entirety of the roughing passes that it calculates from the profile specified between the P and Q blocks, and in essence creates the proper shape of the part. Then as it goes to take a finishing pass it alarms out with an invalid I, J or K in G03. I have had this issue before on smaller parts and was able to play with the numbers until I found values the machine would accept, but that is not working for me this time. This is for a Haas ST35-Y.

  2. #2
    Member
    Join Date
    Jun 2010
    Posts
    3948

    Re: HMC Program Trouble with G03

    Switch to radius mode: it solves a lot of problems.

    Cheers
    Roger

  3. #3
    Flies Fast
    Join Date
    Dec 2008
    Posts
    2818

    Re: HMC Program Trouble with G03

    Your error could be that both I & K need to be stated on all arcs

    N103 would also error as it would use the K-42. value from line N101

    Suggest that all arcs have both addresses stated, and they are modal

  4. #4
    Registered
    Join Date
    Jan 2009
    Posts
    93

    Re: HMC Program Trouble with G03

    without a print or geometry It's hard to help. from what I see the math is wrong.
    try this code and see if it works for you.

    O51712(PRESSURE BLOCK)
    (MATERIAL -YELLOW BRONZE)
    (ORIGIN-X,Y,Z ORIGIN CENTER OF STOCK RADIUS MINUS .150 CLEANUP)
    (TOOLS)
    (TOOL - .200 SQUARE GROOVE TOOL)
    (TOOL -55 DEG)
    G18 G20 G40 G80 G90 G99
    G00 G28
    (55 DEG-FACE AND TURN)
    T101
    G50 S150
    G96 S60 M03
    G00 X18.5 Z.250
    G71 P1 Q2 D.05 U.05 W.05 F.005
    N1 G0 X0.0
    G1 Z0.0 F.005
    G03 X16.5 Z-.81824 K-42.0 (-.8182 CORRECT VALUE FOR END OF ARC @ X16.5)
    G01 X16.5 Z-1.125
    G02 X16.75 Z-1.125 I.0625 ( I.0625 CORRECT FOR X16.5 TO X16.75 DIA.)
    G01 X17.00 Z-1.125
    G01 X17.0 Z-3.0
    N2 G1 X18.5
    G0 X18.5 Z.25
    M00

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
  •