I use 4th positioning most of the time. I don't think i can help cause my code is different from most. I use subs for each tool and have a macro thats codes twice to create the main and sub calls. because we have an okuma, the subs are "called" and are located inside the program rather than an external sub call like on a fanuc. I can pass my tmps on if you have time to learn the syntax. I do have perfect code though. bob code sample below:
$ROTATE.MIN% (ROTATE.MIN) () (PROOFED OUT ? ) (11/02/00) (09:45AM) (EACH PART USES OWN COORD SYS) (EACH PASS THRU SUB INCREMENTS CORD SYS) (X ZERO IS CENTERLINE OF EACH PART) (Y ZERO IS CENTER OF ROTATION) (Z ZERO IS CENTER OF ROTATION) (NOTES:) G15 H1 VC1=1 IF [VATOL EQ 9] NATA T9 M06 (0.266 DIA. TWIST DRILL) (17/64" TITEX JOBBER,A1249) NATA G00 G90 M01 T10 X0.5 Y0.0 CALL OSUBA Q2 G15 H1 VC1=1 IF [VATOL EQ 10] NATB T10 M06 (0.303 DIA. TWIST DRILL) (TITEX LETTER N JOBBER,A1249) NATB G00 G90 M01 T9 X0.1 Y1.0 CALL OSUBB Q2 G15 H1 VC1=1 Z20.0 X0.0 Y20.0 A0.0 VC31=VC31+2 VC32=VC32+2 M02 OSUBA (TOOL 9; 0.266 DIA. TWIST DRILL) (17/64" TITEX JOBBER,A1249) NSA G15 H=VC1 IF [VC1 LE 0] NDA IF [VC1 GT 2] NDA G00 X0.5 Y0.0 S1438 M08 G56 H9 D9 A0.0 ( ROTATION ) Z3.0 M03 G71 Z0.5 G83 Z-0.3119 R0.1 Q0.2 F11.0 M53 G80 M53 M09 Z3.0 VC1=VC1+1 NDA RTS OSUBB (TOOL 10; 0.303 DIA. TWIST DRILL) (TITEX LETTER N JOBBER,A1249) NSB G15 H=VC1 IF [VC1 LE 0] NDB IF [VC1 GT 2] NDB G00 X0.1 Y1.0 S1386 M08 G56 H10 D10 A45.0 ( ROTATION ) Z0.5 M03 G71 Z0.5 G83 Z-0.3119 R0.1 Q0.3 F11.0 M53 G80 M53 M09 Z3.0 VC1=VC1+1 NDB RTS (CYCLE TIME= 0.8 FOR 2.0 PARTS) % -----Original Message----- From: [EMAIL PROTECTED] [mailto:[EMAIL PROTECTED]]On Behalf Of Jon Baker Sent: Thursday, November 02, 2000 9:04 AM To: [EMAIL PROTECTED] Subject: [mfg-smartcam] 4th axis indexing confusion. In the pursuit of 100% perfect code, I have nailed it now on 3 axis machining, however, when I add the 4th axis, I still have a little editing. OK, this is a little anoyance, however, lets see what the smartest smartcam minds can do to help out. Here is my tool change section of my TMP file // TOOL CHANGES @TOOLCHG < #FXD> M9 M5 #MOV G28 G91 Z0 T#TOOL M6 ( #TDESC #TLCMT ) M1 #EVAL(#V9=#SPEED+.2) #EVAL(#CYCLE=jos(cycle)) #IF(#CYCLE=3,#AND#TLTYPE=4)<G0 G17 G40 G80 G90 E1 S#V9 M90 M5>#ELSE<G0 G17 G40 G80 G90 E1> #IF(#CYCLE=3,#AND#TLTYPE=4)< G84.2> #IF(#CYCLE<>3)< #SPNDL S#SPEED> #MOV #IF(#WKSCHG<>1) X#XPOS Y#YPOS A#INDXA #IF(#INDXA<>)< M60 (CLAMP A-AXIS)> G43 H#LOFF D#DOFF #IF(#WKSCHG<>1)< Z#ZPOS>#ELSE< Z#ZHOME> #COOLNT @ Here is my A-axis indexing section // A-AXIS INDEXING @TPINDX ( INDEX TO A#INDXA DEGREES) #MOV #ABSI #FXD Z#ZHOME(CLEARANCE POINT) A#INDXA M60 (A-AXIS BRAKE ON) Here is the code it is putting out N112 T3 M6 ( 1.234 DIA. TWIST DRILL ) N113 M1 N114(STEP DESC.: PILOT DRILL BORE) N115G0 G17 G40 G80 G90 E1 N116 M3 S433 N117 G0 X-0.937 Y0.0 A0.0 N118 M60 (CLAMP A-AXIS) N119 G43 H3 D3 Z3.5 M8 N120 G73 G98 X-0.937 Y0.0 Z-0.25 R2.55 Q1.234 F5.2 N121 ( INDEX TO A180.0 DEGREES) N122 G0 G90 G80 Z3.5(CLEARANCE POINT) N123 A180.0 N124 M60 (A-AXIS BRAKE ON) N125 G73 G98 X-0.937 Y0.0 Z-0.25 R2.55 F5.2 N126 M9 M5 N127 G0 G28 G91 Z0 N128 T4 M6 ( 1.250 DIA. BORE ) N129 M1 N130(STEP DESC.: FINISH BORE) N131G0 G17 G40 G80 G90 E1 N132 M3 S367 N133 G0 X-0.937 Y0.0 A0.0 N134 M60 (CLAMP A-AXIS) N135 G43 H4 D4 Z3.5 M8 N136 ( INDEX TO A0.0 DEGREES) N137 G0 G90 G80 Z3.5(CLEARANCE POINT) N138 A0.0 N139 M60 (A-AXIS BRAKE ON) N140 G88 G98 X-0.937 Y0.0 Z-2.55 R2.55 P500 F1.8 N141 M9 M5 N142 G0 G28 G91 Z0 Now how can I make line 136 thru 139 NOT appear since they already are updated in the tool change. This only happens when I do a tool change AND index to a new A-axis position. I thought the #IF line in the tool change would catch it, but nope. What am I missing. Thanks in advance for your input. Jon ====================================================================== To find out more about this mailing list including how to unsubscribe, send the message "info mfg-smartcam" to [EMAIL PROTECTED] ======================================================================
