509,901 active members
2,958 visitors online
Register for free
Login
IndustryArena Forum > CAM Software > CamWorks > help on toolist EC editor camworks
Results 1 to 9 of 9
  1. #1
    Registered
    Join Date
    Nov 2004
    Posts
    70

    help on toolist EC editor camworks

    i had my toollist post out in the begin of the program, however;
    i need to put the semicolon in front of the bracket of each tool.
    I looKed in the lib. file and master.art mill. file. can't find it. please help

    :C: GETTOOLS(2,SYSTEM)
    POST OUT
    G90 G20
    N2F
    ;N3********* TOOLLIST**********
    ( STATION TOOL TYPE DIAMETER CORNER RADIUS DESCRIPTION )
    ( ------- --------- -------- ------------- -------------------- )
    ( 001 ENDMILL 00.500 .505 RT )
    ( 002 ENDMILL 00.250 .EM )
    N5 G00 G90 G70 G40
    N6G79 Z0
    N7G16XY
    N8M51 M52
    N9M41;M42
    N10;(DAN,YV)
    N11;(UDA,Y/V)
    N12(UTO,1,X-.5,Y.5,Z1)

    THIS IS WHAT I WANT
    ;N3********* TOOLLIST**********
    ;( STATION TOOL TYPE DIAMETER CORNER RADIUS DESCRIPTION )
    ;( ------- --------- -------- ------------- -------------------- )
    ;( 001 ENDMILL 00.500 .505 RT )
    ;( 002 ENDMILL 00.250 .EM )

    SEMICOLON IN FRONT

  2. #2
    Registered
    Join Date
    Feb 2010
    Posts
    60

    Re: help on toolist EC editor camworks

    change your gettools command in the lib,try

    :C: GETTOOLS(2,OUTPUT_TOOL_LIST)

    add a section to configure your output in the .src

    :SECTION=OUTPUT_TOOL_LIST
    :T: <SEMICOLON><LEFT_PAR>T<"%2LNT":TOOL>=<TOOL_COMMENT ><RIGHT_PAR><EOL>

    Add semicolon to your mill.lib file
    :ATTRNAME=SEMICOLON
    :ATTRTYPE=POST
    :ATTREMARK=
    :CODETYPE=HARDCODE
    :CODE=;
    :ATTREND

    Let me know if it worked!

  3. #3
    Registered
    Join Date
    Nov 2004
    Posts
    70

    Re: help on toolist EC editor camworks

    worked perfectly thanks you

  4. #4
    Registered
    Join Date
    Nov 2004
    Posts
    70

    Re: help on toolist EC editor camworks

    HI
    i got my toollist working, moreover; i need to add the tool protrusion ( stickout ) in the tool list help please anybody

    (AKIRA SEIKI 2017)
    (********* TOOLLIST**********)
    ( T01= 5.4MM JOBBER DRILL )
    ( T02= .25 4 FLUTE CRB EM .)

    THIS WHAT IS NEED TO ADD TO THE TOOL LIST
    (AKIRA SEIKI 2017)
    (********* TOOLLIST**********)
    ( T01= 5.4MM JOBBER DRILL . STICKOUT 3.8 )
    ( T02= .25 4 FLUTE CRB EM . STICKOUT 2.5 )




    TOOL_PROTRUSION
    N_TOOL_PROTRUSION
    NC_TOOL_PROTRUSION


    Type
    DECIMAL

    Usage
    This variable stores the tool protrusion from the bottom of the tool holder to the end of a mill tool or a drill tool.





    :ATTRNAME=INI TOOL PROTRUSION
    :ATTRTYPE=POST
    :ATTRVTYPE=DECIMAL
    :ATTREMARK=Z World Coordinate
    :ATTREND

  5. #5
    Registered
    Join Date
    Feb 2010
    Posts
    60

    Re: help on toolist EC editor camworks

    :SECTION=OUTPUT_TOOL_LIST
    :T: <SEMICOLON><LEFT_PAR>T<"%2LNT":TOOL>=<TOOL_COMMENT > STICKOUT <"#1.3":TOOL_PROTRUSION><RIGHT_PAR><EOL>

  6. #6
    Registered
    Join Date
    Nov 2004
    Posts
    70

    Re: help on toolist EC editor camworks

    THANK YOU

  7. #7
    Member
    Join Date
    Nov 2018
    Posts
    4

    EC editor camworks

    Hello I am new to this forum but have been using CamWorks for 5 years and now I have a homemade CNC 5 Axis mill that I need help with federate.

    I am familiar with G93 inverse feed but I want to put that in my .SRC file or I was wondering if I could get help with writing an "IF" command somewhere in the .SRC file. IE (IF A or B THEN F x 5= F) so it would then take the F100 x 5 for F500???

    What happens as you probably know, my rotation is snail speed as F100 in IPM turns to 100 DPM so over 3 1/2 minutes for a full rotation!

    I am also using Mach3 Software to run the mill.
    I have hand edited a file once where I had F100 as the default and every first line of a group that has an A, B move I ended it with F500. I was milling on a .5" Radius part. Any line that did not have an axis move I ended with F100 again.
    That took about 15 entries on a 2000 line file but I want this automated somehow.

    Any help would be appreciated greatly.

  8. #8
    Registered
    Join Date
    Dec 2010
    Posts
    113

    Re: EC editor camworks

    Quote Originally Posted by DJ1 View Post
    Hello I am new to this forum but have been using CamWorks for 5 years and now I have a homemade CNC 5 Axis mill that I need help with federate.

    I am familiar with G93 inverse feed but I want to put that in my .SRC file or I was wondering if I could get help with writing an "IF" command somewhere in the .SRC file. IE (IF A or B THEN F x 5= F) so it would then take the F100 x 5 for F500???

    What happens as you probably know, my rotation is snail speed as F100 in IPM turns to 100 DPM so over 3 1/2 minutes for a full rotation!

    I am also using Mach3 Software to run the mill.
    I have hand edited a file once where I had F100 as the default and every first line of a group that has an A, B move I ended it with F500. I was milling on a .5" Radius part. Any line that did not have an axis move I ended with F100 again.
    That took about 15 entries on a 2000 line file but I want this automated somehow.

    Any help would be appreciated greatly.
    You should start a new topic rather than reviving an old solved one. People will not know to look here for this solution...

    Read these posts for a better understanding of inverse time feed. It is crucial to understanding the math behind it and why your desired solution is not only extremely oversimplified but also potentially dangerous. Simply multiplying the feedrate isn't going to provide predictable results and certainly not so when you get into more complicated situations. You really need to implement the proper math to produce the appropriate desired feedrate.

    Inverse Time Feedrate for 4th Axis
    G93 Inverse Time Feed Move Explained

    Once you have an understanding of how this function truly works, then you can start experimenting with your post. I can't help you much with that aspect other than to point you to the CALC_REG_F section of your GENERAL.LIB file. Copy that section to your <POST>.LIB file and edit it accordingly. It likely already has some comments regarding G94 and G93 feedrates in it. You'll have to decipher how to alter the code logic to determine when to output inverse time feed rates and when not to, and also how to enable it thu the CAMWorks GUI. Post here if you get stuck and I can try to give you more details as you go.

  9. #9
    Member
    Join Date
    Nov 2018
    Posts
    4
    Japazo, Thank you for the quick reply and the .LIB tips, I will check into that.
    I'll read up on the two links you have here also.

Similar Threads

  1. Camworks, UPG, EC Editor: Programming a tool list in Start of Tape
    By Nitan in forum General Off Topic Discussions
    Replies: 1
    Last Post: 12-11-2018, 12:52 PM
  2. Replies: 3
    Last Post: 10-05-2017, 02:03 PM
  3. VB editor
    By RicknBeachcrest in forum Screen Layouts, Post Processors & Misc
    Replies: 2
    Last Post: 07-04-2013, 05:56 PM
  4. MC X Editor
    By cijunet in forum Mastercam
    Replies: 2
    Last Post: 02-21-2008, 05:28 PM
  5. Editor
    By Okuma in forum Uncategorised CAM Discussion
    Replies: 3
    Last Post: 01-07-2004, 02:30 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
  •