Attached is a macro I wrote to automatically do the moves for standard NPT internal pipe threads. I have a pcb file for it but I am at home and it's at work. If anybody really needs it and doesn't know how or wants to tackle writing one (I really don't blame you), let me know and I will get it.
How it works in tm_m.mcl:
#TAP controls the thread size. 0=1/4-18, 1=3/8-18, 2=1/2-14, and
3=3/4-14. It is limited to those four sizes. #CENTERX #CENTERY and #LEVELZ
control the center and top of the location for the thread. #CLEAR is the
clearance plane. #PROF_TOP is the profile top. Cutter compensation is
enabled to the left. I have it set up to create a subroutine if you choose
to go that route (#SUB_ON=1). #NAME controls the name of the subprogram.
At the end of the program I name the entire operation to "RESULT" which then
lets me group it with the macro tm_g.mcl. If I want to undo then I run
tm_u.mcl.
Jeff Guse
----- Original Message -----
From: "Colin Williams" <[EMAIL PROTECTED]>
To: <[EMAIL PROTECTED]>; "Smartcam Forum" <[EMAIL PROTECTED]>
Sent: Friday, June 16, 2000 12:43 PM
Subject: Re: [mfg-smartcam] THREAD MILL
> If you use; process: options: threadmill; in smartcam you don't have to
> worry about cutter comp, it does it for you automatically. I have used it
> for npt threads and it comes out ok. I haven't really been able to get a
> handle what to put in the fields for npt threads.
>
> Colin
> -----Original Message-----
> From: Jeff Brower <[EMAIL PROTECTED]>
> To: Smartcam Forum <[EMAIL PROTECTED]>
> Date: Friday, June 16, 2000 1:23 PM
> Subject: RE: [mfg-smartcam] THREAD MILL
>
>
> >
> >We have always used cutter comp on thread milling operations. I know the
> >book says you can't use comp with helix moves, but it has NEVER failed
> >us...the 'trick' is to add offset comp after creating the helix, since
the
> >helix will not be created with offset no matter what the comp setting is,
> >and to add the lead-in and lead-out moves manually (or create them
first).
> >We've run this way on Fanuc, Mitsubishi, and Haas.
> >
> >We have had trouble with comp and polylines, though. if the line segments
> >are too short and the machine cannot properly comp them. This is a rare
> >case and it always takes a few minutes to catch the problem.
> >
> >another 2 cents,
> >
> >Jeff Brower
> >Stump Preacher Guitars
> >
> >On Friday, June 09, 2000 9:46 AM, Bill Schoeppe [SMTP:[EMAIL PROTECTED]]
> >wrote:
> >> You can program to the edge of the tool if after your done you explode
to
> >a
> >> polyline and put cuttercomp on it.(ONLY SMARTCAM) then do a lead in and
> >out
> >> (Haas Fanuc and fadal all let you run cutter comp in three axis if
every
> >> line has an x,y, in it. ) let smartcam code to the center of the tool
> >and
> >> you will get the most adjustment out of it!!
> >>
> >>
> >> thanks bill
> >>
> >>
> >> -----Original Message-----
> >> From: David Wolfgang <[EMAIL PROTECTED]>
> >> To: Smartcam Forum <[EMAIL PROTECTED]>
> >> Date: Wednesday, June 07, 2000 5:44 PM
> >> Subject: Fw: [mfg-smartcam] THREAD MILL
> >>
> >>
> >> >
> >> >Dave Wolfgang
> >> >----- Original Message -----
> >> >From: "David Wolfgang" <[EMAIL PROTECTED]>
> >> >To: "Colin Williams" <[EMAIL PROTECTED]>
> >> >Sent: Wednesday, June 07, 2000 8:09 PM
> >> >Subject: Re: [mfg-smartcam] THREAD MILL
> >> >
> >> >
> >> >> Major and minor dia are in the machinist handbook for npt threads. I
> >> >program
> >> >> two to three threads deeper than the affective thread depth
(Effective
> >> >> thread depth is the flat on the gauge) but do check the book. Take
the
> >> >> thread minor and add the thread depth is a good starting dia. Then
> >feed
> >> in
> >> >> the + direction at 1 deg. 47' min. Also if you have not programmed
> >thread
> >> >> milling in the past you must program the center of tool path (not
tool
> >> >> edge). good luck.
> >> >>
> >> >> Dave Wolfgang
> >> >>
> >> >> ----- Original Message -----
> >> >> From: "Colin Williams" <[EMAIL PROTECTED]>
> >> >> To: "Smartcam Forum" <[EMAIL PROTECTED]>
> >> >> Sent: Wednesday, June 07, 2000 1:34 PM
> >> >> Subject: [mfg-smartcam] THREAD MILL
> >> >>
> >> >>
> >> >> > PMILL V11.0;
> >> >> >
> >> >> > Using SmartCam "thread mill", I would like to cut a 3/4 - 14 npt,
> >using
> >> >a
> >> >> 4
> >> >> > flute thread mill. The thread mill spec. is .43 dia. at the face
of
> >the
> >> >> tool
> >> >> > with a 1" flute length.
> >> >> >
> >> >> > What diameter would I set my tool to and at what level do I set
to?
> >> Also
> >> >> the
> >> >> > major and minor diameters.
> >> >> >
> >> >> >
> >> >> > Thank You
> >> >> >
> >> >> > Colin Williams
> >> >> > Wabtec Corporation
> >> >> >
> >> >> >
> >> >> >
> >> >> >
> >======================================================================
> >> >> > To find out more about this mailing list including how to
> >unsubscribe,
> >> >> > send the message "info mfg-smartcam" to [EMAIL PROTECTED]
> >> >> >
> >======================================================================
> >> >> >
> >> >>
> >> >
> >> >======================================================================
> >> >To find out more about this mailing list including how to unsubscribe,
> >> >send the message "info mfg-smartcam" to [EMAIL PROTECTED]
> >> >======================================================================
> >> >
> >>
> >> ======================================================================
> >> To find out more about this mailing list including how to unsubscribe,
> >> send the message "info mfg-smartcam" to [EMAIL PROTECTED]
> >> ======================================================================
> >
> >======================================================================
> >To find out more about this mailing list including how to unsubscribe,
> >send the message "info mfg-smartcam" to [EMAIL PROTECTED]
> >======================================================================
>
> ======================================================================
> To find out more about this mailing list including how to unsubscribe,
> send the message "info mfg-smartcam" to [EMAIL PROTECTED]
> ======================================================================
NPT Thread Mill.zip
Description: Zip compressed data
