3dprintforums logo

CNCzone Network:  RFQwork :: 3Dprintforums :: Welderzone :: Google+ :: Our Facebook :: Twitter :: SiteMap



Page 1 of 2 12 LastLast
Results 1 to 12 of 14

Thread: thread milling

  1. #1
    Registered
    Join Date
    Jan 2006
    Location
    USA
    Posts
    328
    Downloads
    0
    Uploads
    0
    Rep Power
    9

    thread milling

    hi guys, I have a trm (cnc 88 control, format 1). I am using solidworks/camworks (2 axis). Sould I be-able to threadmill or is that not possible since I dont have a 3 axis dongle. I would like to have the 3 axis dongle mind you but its a little steep for my blood.


    Mark

    Similar Threads:


  2. #2
    Registered Neal's Avatar
    Join Date
    Mar 2003
    Location
    Chatsworth, Ca
    Posts
    900
    Downloads
    0
    Uploads
    0
    Rep Power
    12

    Smile

    Fourperf--
    Thread milling is simply a three axes helical motion. Here is a sample thread milling prg that does threading on a boss:
    %
    N1O4326(SAMPLE THREAD HOB ON A BOSS
    N2M6T1
    N3G0G90G80G17G40S5000M3E1X2.Y2.
    N4H1Z1.M8
    N5G1Z-0.5F60.
    N6Y0G42
    N7X0F20.
    N8G91G3J-0.5Z-0.0689L6
    N9G90X-2.
    N10G0Z1.
    N11X0Y0Z0H0E0
    N12M2
    %

    Neal



  3. #3
    Registered
    Join Date
    Feb 2007
    Location
    USA
    Posts
    128
    Downloads
    0
    Uploads
    0
    Rep Power
    8
    Thread milling is really quite simple. You can fake it, (add it in by hand)! In a pinch just program a circle then add a z move equal to the thread height like ľ-20, 20 = .050 and thatís your z distance for the whole circle. You just apply this to your roughing & finishing



  4. #4
    Registered
    Join Date
    Jan 2006
    Location
    USA
    Posts
    24
    Downloads
    0
    Uploads
    0
    Rep Power
    0
    For taper thread milling, MMS has a custom macro for machines without the Spiral Interpolation option. www.mmsonline.com/articles/0407cnc.html



  5. #5
    Registered ltmquik's Avatar
    Join Date
    Aug 2005
    Location
    USA
    Posts
    249
    Downloads
    0
    Uploads
    0
    Rep Power
    9
    Quote Originally Posted by fourperf View Post
    hi guys, I have a trm (cnc 88 control, format 1). I am using solidworks/camworks (2 axis). Sould I be-able to threadmill or is that not possible since I dont have a 3 axis dongle. I would like to have the 3 axis dongle mind you but its a little steep for my blood.


    Mark
    You can do all of what the other guys said or in CAMWorks create a boss feature then in the 'attributes' section choose 'THREAD'. You then need to change the settings in the 'parameters' section to the correct thread pitch, generate operations and edit the defs.

    You will also need to make sure that your post is set up to post the z-axis moves. Just double check the code. The nice part about the CAMWorks threadmill is that you can add the cutter comp to the program.

    Jeff Lange
    Lightning Tool & Manufacturing, Inc.


  6. #6
    Registered
    Join Date
    Jan 2006
    Location
    USA
    Posts
    328
    Downloads
    0
    Uploads
    0
    Rep Power
    9
    Quote Originally Posted by ltmquik View Post
    You can do all of what the other guys said or in CAMWorks create a boss feature then in the 'attributes' section choose 'THREAD'. You then need to change the settings in the 'parameters' section to the correct thread pitch, generate operations and edit the defs.

    You will also need to make sure that your post is set up to post the z-axis moves. Just double check the code. The nice part about the CAMWorks threadmill is that you can add the cutter comp to the program.

    I think it must be my post then. I did all you described but when it was run in the machine the machine was moving around the boss but the z was not moving at the same time. The x and y made the correct amound of revolutions around but no simultaneous Z move. I was not sure if I needed to be running 3 axis or not. I guess I simply need to have my reseller adjust my post.

    Mark



  7. #7
    Registered
    Join Date
    Feb 2007
    Location
    USA
    Posts
    128
    Downloads
    0
    Uploads
    0
    Rep Power
    8

    Talking

    I donít think your dilemma constitutes 3 axis machining. And if you look your software is probably 2-1/2 axis not 2. So yes you should be able to thread mill. Almost all software these days give this capability.



  8. #8
    Registered
    Join Date
    Jan 2006
    Location
    USA
    Posts
    328
    Downloads
    0
    Uploads
    0
    Rep Power
    9
    Quote Originally Posted by Big Daddy View Post
    I donít think your dilemma constitutes 3 axis machining. And if you look your software is probably 2-1/2 axis not 2. So yes you should be able to thread mill. Almost all software these days give this capability.
    sorry,my software is in fact 2 1/2 axis. I am away from home now but when I return I am going to see if it my post or if there is something else I was doing wrong.

    Mark

    thanks for the replys



  9. #9
    Registered ltmquik's Avatar
    Join Date
    Aug 2005
    Location
    USA
    Posts
    249
    Downloads
    0
    Uploads
    0
    Rep Power
    9
    Quote Originally Posted by fourperf View Post
    I think it must be my post then. I did all you described but when it was run in the machine the machine was moving around the boss but the z was not moving at the same time. The x and y made the correct amound of revolutions around but no simultaneous Z move. I was not sure if I needed to be running 3 axis or not. I guess I simply need to have my reseller adjust my post.

    Mark
    Mark,
    Check out this for your SRC file.

    :INCLUDE=C:\Program Files\post\millsrc\MILL.T32
    *------------------------------
    :SECTION=START_OF_TAPE
    :T:<O><EOL>
    *
    :SECTION=INIT_TOOL_CHANGE_MILL
    :T:<N><TOOL_COMMENT><EOL>
    :T:<N><T><M:06><EOL>
    *
    *:SECTION=INIT_PRELOAD_TOOL_CHANGE_MILL
    *
    :SECTION=SUB_TOOL_CHANGE_MILL
    :T:<N> Z0 H0<M:05><EOL>
    :T:<N><M:01><EOL>
    :T:<N><T><M:06><EOL>
    :T:<N><TOOL_COMMENT><EOL>
    *
    *:SECTION=SUB_PRELOAD_TOOL_CHANGE_MILL
    *
    :SECTION=FIRST_RAPID_Z_MOVE_DOWN_MILL
    :T:<N><G:90><G:00><Z!> H<"%2LT":TOOL><M:COOLANT_TYPE><EOL>
    *
    *:SECTION=FIRST_RAPID_Z_PRELOAD_DOWN_MILL
    *
    *:SECTION=FIVE_AXIS_FIRST_RAPID_Z_DOWN
    *
    :SECTION=RAPID_Z_MOVE_DOWN_MILL
    :T:<N><G:90><G:00><Z><EOL>
    *
    *:SECTION=FIVE_AXIS_RAPID_Z_MOVE_DOWN
    *
    :SECTION=RAPID_Z_MOVE_UP_MILL
    :T:<N><G:90><G><Z><EOL>
    *
    *:SECTION=FIVE_AXIS_RAPID_Z_MOVE_UP
    *
    :SECTION=LAST_RAPID_Z_MOVE_UP_MILL
    :T:<N><G:90><G><Z><M:09><EOL>
    *
    *:SECTION=FIVE_AXIS_LAST_RAPID_Z_MOVE_UP
    *
    :SECTION=RAPID_FROM_TOOL_CHANGE_MILL
    :T:<N><G!:ABSINC><G!:00><X!><Y!><S!><M!:SPINDLE_DIR><E!>
    :T:<attributes><EOL>
    *
    :SECTION=RAPID_LEADIN_FROM_TOOL_CHANGE_MILL
    :T:<N><G!:ABSINC><G:COMP><G!:00><X!><Y!><S!><M!:SPINDLE_DIR><E!><attributes><EOL>
    *
    *:SECTION=FIVE_AXIS_RAPID_FROM_T_CHANGE
    *
    :SECTION=RAPID_MOVE_MILL
    :T:<N><G:ABSINC><G:00><X><Y><E><attributes><EOL>
    *
    :SECTION=RAPID_LEADIN_MOVE_MILL
    :T:<N><G:ABSINC><G:COMP><G:00><X><Y><E><attributes><EOL>
    *
    :SECTION=RAPID_LEADOUT_MOVE_MILL
    :T:<N><G:ABSINC><G:40><G:00><X!><Y!><E><attributes><EOL>
    *
    *:SECTION=FIVE_AXIS_RAPID_MOVE_MILL
    *
    *:SECTION=RAPID_TO_TOOL_CHANGE_MILL
    *
    *:SECTION=RAPID_LEADOUT_TO_TOOL_CHANGE_MILL
    *
    *:SECTION=FIVE_AXIS_RAPID_TO_T_CHANGE
    *
    :SECTION=FEED_Z_MOVE_DOWN_MILL
    :T:<N><G:90><G:01><Z><F><EOL>
    *
    *:SECTION=FIVE_AXIS_FEED_Z_MOVE_DOWN
    *
    :SECTION=LINE_LEADIN_MOVE_MILL
    :T:<N><G:ABSINC><G:COMP><COMP_NUMBER><G:01><X!><Y!><Z><F><attributes><EOL>
    *
    :SECTION=LINE_MOVE_MILL
    :T:<N><G:ABSINC><G:01><X><Y><Z><F><attributes><EOL>
    *
    *:SECTION=FASTLINE
    *
    *:SECTION=FIVE_AXIS_LINE_MOVE_MILL
    *
    :SECTION=LINE_LEADOUT_MOVE_MILL
    :T:<N><G:ABSINC><G:40><G:01><X><Y><Z><F><EOL>
    *
    :SECTION=ARC_MOVE_MILL
    :T:<N><G:ARC_DIR><X><Y><Z><I><J><F><EOL>
    *
    :SECTION=RADIUS_MOVE_MILL
    :T:<N><G:ABSINC><G><X><Y><R><F><attributes><EOL>
    *
    :SECTION=DRILL_POSITION
    :T:<N><G!:ABSINC><G!:00><X!><Y!><S!><M!:SPINDLE_DIR><E!><attributes><EOL>
    *
    :SECTION=DRILLING_CYCLE
    :T:<N><G:ABSINC><G:81><G:PLANE><X!><Y!><Z_CLEAR><Z_DEPTH><F><M:COOLANT_TYPE><EOL>
    *
    :SECTION=SPOT_DRILLING_CYCLE
    :T:<N><G:ABSINC><G:82><G:PLANE><X!><Y!><Z_CLEAR><Z_DEPTH> P<%dwell*1000)><F><M:COOLANT_TYPE><EOL>
    *
    :SECTION=PECKING_CYCLE
    :T:<N><G:ABSINC><G:83><G:PLANE><X!><Y!><Z_CLEAR><Z_DEPTH><SUB_PECK><F><M:COOLANT_TYPE><EOL>
    *
    :SECTION=VARIABLE_PECKING_CYCLE
    :T:<N><G:ABSINC><G:83><G:PLANE><X!><Y!><Z_CLEAR><Z_DEPTH> I<#:OPR_Z_FIRST_PECK>
    :T: J<#ABS(OPR_Z_FIRST_PECK-OPR_Z_SUB_PECK))> K<#:minimum_increment><F><M:COOLANT_TYPE><EOL>
    *
    :SECTION=TAPPING_CYCLE
    :T:<N><G:ABSINC><G:84><G:PLANE><X!><Y!><Z_CLEAR><Z_DEPTH> Q<"#3.4":OPR_Z_FEED>
    :T:<F!OPR_SPEED+.2)><M:COOLANT_TYPE><EOL>


    Be sure you have the 'Z' in the SECTION=ARC_MILL_MOVE and the SECTION=LINE_MILL_MOVE.

    Jeff Lange
    Lightning Tool & Manufacturing, Inc.


  10. #10
    Registered ltmquik's Avatar
    Join Date
    Aug 2005
    Location
    USA
    Posts
    249
    Downloads
    0
    Uploads
    0
    Rep Power
    9
    Mark,
    You can also e-mail me the SRC and LIB files and I will adjust your post.

    Jeff Lange
    Lightning Tool & Manufacturing, Inc.


  11. #11
    Registered
    Join Date
    Jan 2006
    Location
    USA
    Posts
    328
    Downloads
    0
    Uploads
    0
    Rep Power
    9
    thanks a lot Jeff, Thats really helpful. I will check that when I get home. Thanks for doing that

    Mark



  12. #12
    Registered ltmquik's Avatar
    Join Date
    Aug 2005
    Location
    USA
    Posts
    249
    Downloads
    0
    Uploads
    0
    Rep Power
    9
    Quote Originally Posted by fourperf View Post
    thanks a lot Jeff, Thats really helpful. I will check that when I get home. Thanks for doing that

    Mark
    Mark,
    I just noticed that the site post some silly unhappy faces in the code. These should be replaced by a colon ":".

    Jeff Lange
    Lightning Tool & Manufacturing, Inc.


Page 1 of 2 12 LastLast

Tags for this Thread

Posting Permissions



About CNCzone.com

    We are the largest and most active discussion forum from DIY CNC Machines to the Cad/Cam software to run them. The site is 100% free to join and use, so join today!

Follow us on

Facebook Dribbble RSS Feed