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

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

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 ¼-20, 20 = .050 and that’s your z distance for the whole circle. You just apply this to your roughing & finishing

For taper thread milling, MMS has a custom macro for machines without the Spiral Interpolation option. www.mmsonline.com/articles/0407cnc.html

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.

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

I don’t 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.

I don’t 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

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.

Mark,
You can also e-mail me the SRC and LIB files and I will adjust your post.

thanks a lot Jeff, Thats really helpful. I will check that when I get home. Thanks for doing that

Mark

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 ":".

Mark,
You can also e-mail me the SRC and LIB files and I will adjust your post.


Thank you so much Jeff. I would really appreciate that. I will be home the middle of June and send you and E mail.

Mark

Hi
I am having the same problem, I need to program 2 3" - 8 npt pockets (internal threading), 1" deep using a single edge, boring bar style cutter. The control is an old CNC 88, and I'm using Mastercam ver. 9. Any ideas. I got it programmed, but it was over 1,000 lines of g-code, and the control said "No thanks".

Thanks
John