Your canned cycles will depend on the model fanuc you have. I have not had much luck in using turning canned cycles. There is only two advantages to using canned cycles for the lathe. One you can change the depth of cut in roughing with just changing one number. And two it takes alot less space in your machines memory. When I need those advantages I put it in using the user command. Here is my G76 Thread cycle for Fanuc OT @FXD1 #IF(#U1=0)<#EVAL(#U1=2)> #IF(#U2=0)<#EVAL(#U2=2)> #IF(#U3=0)<#EVAL(#U3=29)> #IF(#U4=0)<#EVAL(#U4=.001)> #IF(#U5=0)<#EVAL(#U5=.0005)> G76 P#FMT(#U1,F2.0)#FMT(#U2,F2.0)#FMT(#U3,F2.0) Q#FMT(#U4,T1.4)#EXLN R#FMT(#U5,T1.4) G76 X#XPASS Z#ZPASS#EXLN < R#FMT(#XOV,T1.4)> P#FMT(#V1,T1.4) Q#FMT(#V2,T1.4) F#FMT(#FTHRD,D1.6)
Also your Tap cycle needs help @FXD4 G32 Z#ZPASS F#FMT(#FTHRD,D1.6) #SPNDL M5 #IF(#SPNDL=1)<#EVAL(#SPNDL=2)>#ELSE<#EVAL(#SPNDL=1)> G32 Z#ZPOS F#FMT(#FTHRD,D1.6) #SPNDL Good luck in Using SmartCam I'm sure you will like it and the versatility. Dave Wolfgang ----- Original Message ----- From: "Wojciech" <[EMAIL PROTECTED]> To: "SmartCAM Mailing List" <[EMAIL PROTECTED]> Sent: Saturday, October 14, 2000 7:19 PM Subject: [mfg-smartcam] Code Generator for Daewoo Lynx with Fanuc Control > I'm just starting using Smartcam so I wanted to customize code > generator. I'm going to use it mostly on Daewoo machines with Fanuc > Control. I've started with lathe.tmp file that comes with the > software. I wanted to get rid of the line numbering, change I/K to R > in G02/G03 and couple other things. Beneath is what I've got. What do > you think about it? Is it error free? > > __________ > > @START > <#OFFBLK> > % > :O0000(#FILE) > G20G40G99 > N#FMT(#TOOL,T2.0)( #TDESC ) > G00X6.0Z6.0 > G00T#TOFF > G50S2000 > #SPMODE<S#SPEED>#SPNDL > M08 > #NEXTPT > #MOV<X#XPOS>Z#ZPOS > > @TOOLCHG > G00X6.0Z6.0M09 > M01 > N#FMT(#TOOL,T2.0)( #TDESC ) > G00X6.0Z6.0 > T#TOFF > G50S2000 > #SPMODE<S#SPEED>#SPNDL > M08 > #NEXTPT > #MOV<X#XPOS>Z#ZPOS > > @END > G00X6.0Z6.0M09 > M01 > M30 > #OFFBLK% > > @STPROF > <#MOV><X#XPOS><Z#ZPOS> > > @RAP > <#MOV><X#XPOS><Z#ZPOS> > > @LINE > <#MOV><X#XPOS><Z#ZPOS><F#FEED> > > @ARC > <#MOV><X#XPOS><Z#ZPOS><R#ARAD><F#FEED> > > @FXD1 > G33<X#XPOS><Z#ZPOS><F#FTHRD> > > @FXD4 > G33<Z#ZPASS><F#FEED> > M03 > G33<Z#ZPOS><F#FEED> > @ > __________ > > > > In other file I found those codes: > ________ > @FXD1 > #EVAL(#V1=ABS(#V1)) > #EVAL(#V2=ABS(#V2)) > #IF(#XPASS<#XCTR)<#EVAL(#XOV=ABS(#XOV))> > G76X#XPASSZ#ZPASS<I#XOV>K#V1D#V2F#FTHRDA#U0<#C1> > > @FXD2 > <#FXD><X#XPASS><Z#ZPASS><#C1><F#FEED> > > @FXD3 > <#FXD><X#XPASS><Z#ZPASS><#C1><F#FEED> > > @FXD4 > G33Z#ZPASS<F#FEED> > M05 > M04 > G33Z#ZPOS<F#FEED> > M05 > > @DWELL > G04U#DWELL#EVAL(#TIME=#DWELL/60) > > @RTURN > #RESET(#MOV) > #EVAL(#U2=#BLK+1) > G71P#U2Q#U3U#V3W#V4D#V5F#FEEDS#SPEED<#C1> > #NEXTPT > > @RFACE > #RESET(#MOV) > #EVAL(#U1=#BLK+1) > G72P#U2Q#U3U#V3W#V4D#V5F#FEEDS#SPEED<#C1> > #NEXTPT > > @FTURN > G70P#U2Q#U3 > > @REND > #EVAL(#U3=#BLK-1) > ________ > > Can I put it in my file so Smartcam would be using G71/G72 for > roughing and G76 for threading? I'm not sure what <#C1> do in it. Does > it have anything to do with tool radius compensation? Can I just > delete it from those lines if I work only in G40 mode? > THX for opinions. > > -- > > _| _| _|_| _| _| _|_|_| _|_| > _| _| _| _| _| _| _| _| _| > _| _| _| _| _|_| _| _|_| > _|_| _| _| _| _| _| _| > _| _|_| _| _| _|_| > > @Yahoo.com > > > > _________________________________________________________ > Do You Yahoo!? > Get your free @yahoo.com address at http://mail.yahoo.com > > ====================================================================== > 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] ======================================================================
