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] ======================================================================
