Thread: Machining order

**pp-TG** · 09-04-2013, 03:10 AM

I have 3 machine setups G54, G55 and G56. I am using tools that work on all three. So lets say I have to drill and tap a 1/4-20 hole on all three work shifts when I post this it does use each tool (spot drill, drill, and tap) on each work shift before going to the next tool but it always returns to G54. So it will spot drill on G54 then G55 then G56 then it will call up the drill and go back to G54 instead of working backwards or staying on the work shift it is on. This happens with end mills and pockets also. Is there a way to fix this?

**aldepoalo** · 09-04-2013, 03:28 PM

Attachment 199116

In the V25 you have 3 options for posting order.

If you want the software to post the center drill for all setups then you would choose individual Tool. At this time it post the work offset in order 54,55,56 but it would be nice to have it post in reverse order to run parts faster. Same with drilling holes in a single setup....

Here is a sample program to spot drill, drill, and chamfer on 3 work offsets:

Posting by Feature:

Code:

%
O100 (PROGRAM NUMBER)

(BEGIN PREDATOR NC HEADER)
(MCH_FILE=4AXVMILL.MCH)
(COORD_SYS 1=X0 Y0 Z0)
(MTOOL T1 S4 D0.5 C0. A90. H3.)
(MTOOL T2 S4 D0.5 C0. A118. H6.)
(MTOOL T3 S7 D0.75 C0. A90. H3.5)
(MTOOL T4 S7 D0.875 C0.125 A90. H5.)
(MTOOL T5 S7 D1. C0.125 A90. H5.)
(SBOX X0. Y0. Z-1. L6.1445 W5.8431 H1.)
(END PREDATOR NC HEADER)


(FIRST MACHINE SETUP - Machine Setup - 1)

(PROGRAM NAME - BOBCAD2.NC)
(POST -  HAAS VF)
(DATE - WED. 09/04/2013)
(TIME - 10:26AM)

N01 G00 G17 G40 G49 G80 G20 G90

(FIRST CUT - FIRST TOOL)
(JOB 1  HOLE  RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)

(TOOL #1 0.5  1/2 - 90 DEGREE SPOT DRILL)
N02 T1 M06
N03 G90 G54 X0.9065 Y0.6715 S3880 M03
N04 G43 H1 D1 Z0.1 M08
N05 G81 G99 X0.9065 Y0.6715 Z-0.08 R0.1 F11.1574
N06 G80
N07 M09
N08 M05
N09 G00 G91 G28 Z0.
N10 M01

(NEXT CUT - NEXT TOOL)
(JOB 1  HOLE  RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)

(TOOL #2 1/2 DRILL)
N11 T2 M06
N12 G90 G54 X0.9065 Y0.6715 S3880 M03
N13 G43 H2 D2 Z0.1 M08
N14 G81 G99 X0.9065 Y0.6715 Z-0.6502 R0.1 F22.3148
N15 G80
N16 M09
N17 M05
N18 G00 G91 G28 Z0.
N19 M01

(NEXT CUT - NEXT TOOL)
(JOB 1  HOLE  RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)

(TOOL #3 3/4 - Sharp Chamfer Tool)
N20 T3 M06
N21 G90 G54 X0.9065 Y0.6715 S2587 M03
N22 G43 H3 D3 Z0.1 M08
N23 G81 G99 X0.9065 Y0.6715 Z-0.27 R0.1 F7.4383
N24 G80

N25 M00
(NEXT MACHINE SETUP - Machine Setup - 2)

N26 M09
N27 M05
N28 G00 G91 G28 Z0.
N29 M01

(NEXT CUT - NEXT TOOL)
(JOB 2  HOLE  RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)

(TOOL #1 1/2 - 90 DEGREE SPOT DRILL)
N30 T1 M06
N31 G90 G55 X-1.2189 Y0.6532 S3880 M03
N32 G43 H1 D1 Z0.1 M08
N33 G81 G99 X-1.2189 Y0.6532 Z-0.08 R0.1 F11.1574
N34 G80
N35 M09
N36 M05
N37 G00 G91 G28 Z0.
N38 M01

(NEXT CUT - NEXT TOOL)
(JOB 2  HOLE  RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)

(TOOL #2 1/2 DRILL)
N39 T2 M06
N40 G90 G55 X-1.2189 Y0.6532 S3880 M03
N41 G43 H2 D2 Z0.1 M08
N42 G81 G99 X-1.2189 Y0.6532 Z-0.6502 R0.1 F22.3148
N43 G80
N44 M09
N45 M05
N46 G00 G91 G28 Z0.
N47 M01

(NEXT CUT - NEXT TOOL)
(JOB 2  HOLE  RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)

(TOOL #4 90.0000 Deg. 0.8750 Dia.0.1250 SmDia.)
N48 T4 M06
N49 G90 G55 X-1.2189 Y0.6532 S2217 M03
N50 G43 H4 D4 Z0.1 M08
N51 G81 G99 X-1.2189 Y0.6532 Z-0.3375 R0.1 F6.3757
N52 G80

N53 M00
(NEXT MACHINE SETUP - Machine Setup - 3)

N54 M09
N55 M05
N56 G00 G91 G28 Z0.
N57 M01

(NEXT CUT - NEXT TOOL)
(JOB 3  HOLE  RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)

(TOOL #1 1/2 - 90 DEGREE SPOT DRILL)
N58 T1 M06
N59 G90 G56 X1.2156 Y0.6871 S3880 M03
N60 G43 H1 D1 Z0.1 M08
N61 G81 G99 X1.2156 Y0.6871 Z-0.08 R0.1 F11.1574
N62 G80
N63 M09
N64 M05
N65 G00 G91 G28 Z0.
N66 M01

(NEXT CUT - NEXT TOOL)
(JOB 3  HOLE  RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)

(TOOL #2 1/2 DRILL)
N67 T2 M06
N68 G90 G56 X1.2156 Y0.6871 S3880 M03
N69 G43 H2 D2 Z0.1 M08
N70 G81 G99 X1.2156 Y0.6871 Z-0.6502 R0.1 F22.3148
N71 G80
N72 M09
N73 M05
N74 G00 G91 G28 Z0.
N75 M01

(NEXT CUT - NEXT TOOL)
(JOB 3  HOLE  RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)

(TOOL #5 90.0000 Deg. 1.0000 Dia.0.1250 SmDia.)
N76 T5 M06
N77 G90 G56 X1.2156 Y0.6871 S1940 M03
N78 G43 H5 D5 Z0.1 M08
N79 G81 G99 X1.2156 Y0.6871 Z-0.4 R0.1 F5.5787
N80 G80
N81 M09
N82 M05
N83 G00 G91 G28 Z0.
N84 G91 G28 Y0.
N85 T1 M06
N86 M02

(END OF FILE)
(END OF PROGRAM)

N87 M30
%

Posting by Individual Tool Per Setup:

Code:

%
O100 (PROGRAM NUMBER)

(BEGIN PREDATOR NC HEADER)
(MCH_FILE=4AXVMILL.MCH)
(COORD_SYS 1=X0 Y0 Z0)
(MTOOL T1 S4 D0.5 C0. A90. H3.)
(MTOOL T2 S4 D0.5 C0. A118. H6.)
(MTOOL T3 S7 D0.75 C0. A90. H3.5)
(MTOOL T4 S7 D0.875 C0.125 A90. H5.)
(MTOOL T5 S7 D1. C0.125 A90. H5.)
(SBOX X0. Y0. Z-1. L6.1445 W5.8431 H1.)
(END PREDATOR NC HEADER)


(FIRST MACHINE SETUP - Machine Setup - 1)

(PROGRAM NAME - BOBCAD2.NC)
(POST -  HAAS VF)
(DATE - WED. 09/04/2013)
(TIME - 10:27AM)

N01 G00 G17 G40 G49 G80 G20 G90

(FIRST CUT - FIRST TOOL)
(JOB 1  HOLE  RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)

(TOOL #1 0.5  1/2 - 90 DEGREE SPOT DRILL)
N02 T1 M06
N03 G90 G54 X0.9065 Y0.6715 S3880 M03
N04 G43 H1 D1 Z0.1 M08
N05 G81 G99 X0.9065 Y0.6715 Z-0.08 R0.1 F11.1574
N06 G80
N07 M09
N08 M05
N09 G00 G91 G28 Z0.
N10 M01

(NEXT CUT - NEXT TOOL)
(JOB 1  HOLE  RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)

(TOOL #2 1/2 DRILL)
N11 T2 M06
N12 G90 G54 X0.9065 Y0.6715 S3880 M03
N13 G43 H2 D2 Z0.1 M08
N14 G81 G99 X0.9065 Y0.6715 Z-0.6502 R0.1 F22.3148
N15 G80
N16 M09
N17 M05
N18 G00 G91 G28 Z0.
N19 M01

(NEXT CUT - NEXT TOOL)
(JOB 1  HOLE  RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)

(TOOL #3 3/4 - Sharp Chamfer Tool)
N20 T3 M06
N21 G90 G54 X0.9065 Y0.6715 S2587 M03
N22 G43 H3 D3 Z0.1 M08
N23 G81 G99 X0.9065 Y0.6715 Z-0.27 R0.1 F7.4383
N24 G80

N25 M00
(NEXT MACHINE SETUP - Machine Setup - 2)

N26 M09
N27 M05
N28 G00 G91 G28 Z0.
N29 M01

(NEXT CUT - NEXT TOOL)
(JOB 2  HOLE  RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)

(TOOL #1 1/2 - 90 DEGREE SPOT DRILL)
N30 T1 M06
N31 G90 G55 X-1.2189 Y0.6532 S3880 M03
N32 G43 H1 D1 Z0.1 M08
N33 G81 G99 X-1.2189 Y0.6532 Z-0.08 R0.1 F11.1574
N34 G80
N35 M09
N36 M05
N37 G00 G91 G28 Z0.
N38 M01

(NEXT CUT - NEXT TOOL)
(JOB 2  HOLE  RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)

(TOOL #2 1/2 DRILL)
N39 T2 M06
N40 G90 G55 X-1.2189 Y0.6532 S3880 M03
N41 G43 H2 D2 Z0.1 M08
N42 G81 G99 X-1.2189 Y0.6532 Z-0.6502 R0.1 F22.3148
N43 G80
N44 M09
N45 M05
N46 G00 G91 G28 Z0.
N47 M01

(NEXT CUT - NEXT TOOL)
(JOB 2  HOLE  RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)

(TOOL #4 90.0000 Deg. 0.8750 Dia.0.1250 SmDia.)
N48 T4 M06
N49 G90 G55 X-1.2189 Y0.6532 S2217 M03
N50 G43 H4 D4 Z0.1 M08
N51 G81 G99 X-1.2189 Y0.6532 Z-0.3375 R0.1 F6.3757
N52 G80

N53 M00
(NEXT MACHINE SETUP - Machine Setup - 3)

N54 M09
N55 M05
N56 G00 G91 G28 Z0.
N57 M01

(NEXT CUT - NEXT TOOL)
(JOB 3  HOLE  RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)

(TOOL #1 1/2 - 90 DEGREE SPOT DRILL)
N58 T1 M06
N59 G90 G56 X1.2156 Y0.6871 S3880 M03
N60 G43 H1 D1 Z0.1 M08
N61 G81 G99 X1.2156 Y0.6871 Z-0.08 R0.1 F11.1574
N62 G80
N63 M09
N64 M05
N65 G00 G91 G28 Z0.
N66 M01

(NEXT CUT - NEXT TOOL)
(JOB 3  HOLE  RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)

(TOOL #2 1/2 DRILL)
N67 T2 M06
N68 G90 G56 X1.2156 Y0.6871 S3880 M03
N69 G43 H2 D2 Z0.1 M08
N70 G81 G99 X1.2156 Y0.6871 Z-0.6502 R0.1 F22.3148
N71 G80
N72 M09
N73 M05
N74 G00 G91 G28 Z0.
N75 M01

(NEXT CUT - NEXT TOOL)
(JOB 3  HOLE  RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)

(TOOL #5 90.0000 Deg. 1.0000 Dia.0.1250 SmDia.)
N76 T5 M06
N77 G90 G56 X1.2156 Y0.6871 S1940 M03
N78 G43 H5 D5 Z0.1 M08
N79 G81 G99 X1.2156 Y0.6871 Z-0.4 R0.1 F5.5787
N80 G80
N81 M09
N82 M05
N83 G00 G91 G28 Z0.
N84 G91 G28 Y0.
N85 T1 M06
N86 M02

(END OF FILE)
(END OF PROGRAM)

N87 M30
%

Posting by Individual Tool:

Code:

%
O100 (PROGRAM NUMBER)

(BEGIN PREDATOR NC HEADER)
(MCH_FILE=4AXVMILL.MCH)
(COORD_SYS 1=X0 Y0 Z0)
(MTOOL T1 S4 D0.5 C0. A90. H3.)
(MTOOL T2 S4 D0.5 C0. A118. H6.)
(MTOOL T3 S7 D0.75 C0. A90. H3.5)
(MTOOL T4 S7 D0.875 C0.125 A90. H5.)
(MTOOL T5 S7 D1. C0.125 A90. H5.)
(SBOX X0. Y0. Z-1. L6.1445 W5.8431 H1.)
(END PREDATOR NC HEADER)


(FIRST MACHINE SETUP - Machine Setup - 1)

(PROGRAM NAME - BOBCAD2.NC)
(POST -  HAAS VF)
(DATE - WED. 09/04/2013)
(TIME - 10:27AM)

N01 G00 G17 G40 G49 G80 G20 G90

(FIRST CUT - FIRST TOOL)
(JOB 1  HOLE  RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)

(TOOL #1 0.5  1/2 - 90 DEGREE SPOT DRILL)
N02 T1 M06
N03 G90 G54 X0.9065 Y0.6715 S3880 M03
N04 G43 H1 D1 Z0.1 M08
N05 G81 G99 X0.9065 Y0.6715 Z-0.08 R0.1 F11.1574
N06 G80

N07 M00
(NEXT MACHINE SETUP - Machine Setup - 2)


(NEXT CUT - SAME TOOL)
(JOB 2  HOLE  RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)

N08 G00 X-1.2189 Y0.6532 S3880
N09 G81 G99 X-1.2189 Y0.6532 Z-0.08 R0.1 F11.1574
N10 G80

N11 M00
(NEXT MACHINE SETUP - Machine Setup - 3)


(NEXT CUT - SAME TOOL)
(JOB 3  HOLE  RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)

N12 G00 X1.2156 Y0.6871 S3880
N13 G81 G99 X1.2156 Y0.6871 Z-0.08 R0.1 F11.1574
N14 G80

N15 M00
(NEXT MACHINE SETUP - Machine Setup - 1)

N16 M09
N17 M05
N18 G00 G91 G28 Z0.
N19 M01

(NEXT CUT - NEXT TOOL)
(JOB 1  HOLE  RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)

(TOOL #2 1/2 DRILL)
N20 T2 M06
N21 G90 G54 X0.9065 Y0.6715 S3880 M03
N22 G43 H2 D2 Z0.1 M08
N23 G81 G99 X0.9065 Y0.6715 Z-0.6502 R0.1 F22.3148
N24 G80

N25 M00
(NEXT MACHINE SETUP - Machine Setup - 2)


(NEXT CUT - SAME TOOL)
(JOB 2  HOLE  RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)

N26 G00 X-1.2189 Y0.6532 S3880
N27 G81 G99 X-1.2189 Y0.6532 Z-0.6502 R0.1 F22.3148
N28 G80

N29 M00
(NEXT MACHINE SETUP - Machine Setup - 3)


(NEXT CUT - SAME TOOL)
(JOB 3  HOLE  RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)

N30 G00 X1.2156 Y0.6871 S3880
N31 G81 G99 X1.2156 Y0.6871 Z-0.6502 R0.1 F22.3148
N32 G80

N33 M00
(NEXT MACHINE SETUP - Machine Setup - 1)

N34 M09
N35 M05
N36 G00 G91 G28 Z0.
N37 M01

(NEXT CUT - NEXT TOOL)
(JOB 1  HOLE  RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)

(TOOL #3 3/4 - Sharp Chamfer Tool)
N38 T3 M06
N39 G90 G54 X0.9065 Y0.6715 S2587 M03
N40 G43 H3 D3 Z0.1 M08
N41 G81 G99 X0.9065 Y0.6715 Z-0.27 R0.1 F7.4383
N42 G80

N43 M00
(NEXT MACHINE SETUP - Machine Setup - 2)

N44 M09
N45 M05
N46 G00 G91 G28 Z0.
N47 M01

(NEXT CUT - NEXT TOOL)
(JOB 2  HOLE  RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)

(TOOL #4 90.0000 Deg. 0.8750 Dia.0.1250 SmDia.)
N48 T4 M06
N49 G90 G55 X-1.2189 Y0.6532 S2217 M03
N50 G43 H4 D4 Z0.1 M08
N51 G81 G99 X-1.2189 Y0.6532 Z-0.3375 R0.1 F6.3757
N52 G80

N53 M00
(NEXT MACHINE SETUP - Machine Setup - 3)

N54 M09
N55 M05
N56 G00 G91 G28 Z0.
N57 M01

(NEXT CUT - NEXT TOOL)
(JOB 3  HOLE  RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)

(TOOL #5 90.0000 Deg. 1.0000 Dia.0.1250 SmDia.)
N58 T5 M06
N59 G90 G56 X1.2156 Y0.6871 S1940 M03
N60 G43 H5 D5 Z0.1 M08
N61 G81 G99 X1.2156 Y0.6871 Z-0.4 R0.1 F5.5787
N62 G80
N63 M09
N64 M05
N65 G00 G91 G28 Z0.
N66 G91 G28 Y0.
N67 T1 M06
N68 M02

(END OF FILE)
(END OF PROGRAM)

N69 M30
%

*** Just noticed my post is not setup correctly to post this properly.... you can see the M00 but you don't see the change in work offset... Simple fix in the post. I think I would want to add a work offset call and zr in the null tool change block for post the work offset and an rapid to clearance move between features.....

More like this:

Code:

%
O100 (PROGRAM NUMBER)

(BEGIN PREDATOR NC HEADER)
(MCH_FILE=4AXVMILL.MCH)
(COORD_SYS 1=X0 Y0 Z0)
(MTOOL T1 S4 D0.5 C0. A90. H3.)
(MTOOL T2 S4 D0.5 C0. A118. H6.)
(MTOOL T3 S7 D0.75 C0. A90. H3.5)
(SBOX X0. Y0. Z-1. L6.1445 W5.8431 H1.)
(END PREDATOR NC HEADER)


(FIRST MACHINE SETUP - Machine Setup - 1)

(PROGRAM NAME - BOBCAD2.NC)
(POST -  HAAS VF)
(DATE - WED. 09/04/2013)
(TIME - 11:23AM)

N01 G00 G17 G40 G49 G80 G20 G90

(FIRST CUT - FIRST TOOL)
(JOB 1  HOLE  RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)

(TOOL #1 0.5  1/2 - 90 DEGREE SPOT DRILL)
N02 T1 M06
N03 G90 G54 X0.9065 Y0.6715 S3880 M03
N04 G43 H1 D1 Z0.1 M08
N05 G81 G99 X0.9065 Y0.6715 Z-0.08 R0.1 F11.1574
N06 G80

N07 M01
(NEXT MACHINE SETUP - Machine Setup - 2)


(NEXT CUT - SAME TOOL)
(JOB 2  HOLE  RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)

N08 G55 G00 Z0.1
N09 G00 X-1.2189 Y0.6532 S3880
N10 G81 G99 X-1.2189 Y0.6532 Z-0.08 R0.1 F11.1574
N11 G80

N12 M01
(NEXT MACHINE SETUP - Machine Setup - 3)


(NEXT CUT - SAME TOOL)
(JOB 3  HOLE  RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)

N13 G56 G00 Z0.1
N14 G00 X1.2156 Y0.6871 S3880
N15 G81 G99 X1.2156 Y0.6871 Z-0.08 R0.1 F11.1574
N16 G80

N17 M01
(NEXT MACHINE SETUP - Machine Setup - 1)

N18 M09
N19 M05
N20 G00 G91 G28 Z0.
N21 M01

(NEXT CUT - NEXT TOOL)
(JOB 1  HOLE  RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)

(TOOL #2 1/2 DRILL)
N22 T2 M06
N23 G90 G54 X0.9065 Y0.6715 S3880 M03
N24 G43 H2 D2 Z0.1 M08
N25 G81 G99 X0.9065 Y0.6715 Z-0.6502 R0.1 F22.3148
N26 G80

N27 M01
(NEXT MACHINE SETUP - Machine Setup - 2)


(NEXT CUT - SAME TOOL)
(JOB 2  HOLE  RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)

N28 G55 G00 Z0.1
N29 G00 X-1.2189 Y0.6532 S3880
N30 G81 G99 X-1.2189 Y0.6532 Z-0.6502 R0.1 F22.3148
N31 G80

N32 M01
(NEXT MACHINE SETUP - Machine Setup - 3)


(NEXT CUT - SAME TOOL)
(JOB 3  HOLE  RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)

N33 G56 G00 Z0.1
N34 G00 X1.2156 Y0.6871 S3880
N35 G81 G99 X1.2156 Y0.6871 Z-0.6502 R0.1 F22.3148
N36 G80

N37 M01
(NEXT MACHINE SETUP - Machine Setup - 1)

N38 M09
N39 M05
N40 G00 G91 G28 Z0.
N41 M01

(NEXT CUT - NEXT TOOL)
(JOB 1  HOLE  RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)

(TOOL #3 3/4 - Sharp Chamfer Tool)
N42 T3 M06
N43 G90 G54 X0.9065 Y0.6715 S2587 M03
N44 G43 H3 D3 Z0.1 M08
N45 G81 G99 X0.9065 Y0.6715 Z-0.27 R0.1 F7.4383
N46 G80

N47 M01
(NEXT MACHINE SETUP - Machine Setup - 2)


(NEXT CUT - SAME TOOL)
(JOB 2  HOLE  RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)

N48 G55 G00 Z0.1
N49 G00 X-1.2189 Y0.6532 S2217
N50 G81 G99 X-1.2189 Y0.6532 Z-0.3375 R0.1 F6.3757
N51 G80

N52 M01
(NEXT MACHINE SETUP - Machine Setup - 3)


(NEXT CUT - SAME TOOL)
(JOB 3  HOLE  RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)

N53 G56 G00 Z0.1
N54 G00 X1.2156 Y0.6871 S1940
N55 G81 G99 X1.2156 Y0.6871 Z-0.4 R0.1 F5.5787
N56 G80
N57 M09
N58 M05
N59 G00 G91 G28 Z0.
N60 G91 G28 Y0.
N61 T1 M06
N62 M02

(END OF FILE)
(END OF PROGRAM)

N63 M30
%

**SBC Cycle** · 09-04-2013, 04:45 PM

I'm thinking he is looking for something like option 3 (by Tool) but instead of going:

Center Drill: G54 G55 G56
Drill: G54 G55 G56
Tap: G54 G55 G56

Center Drill: G54 G55 G56
Drill: G56 G55 G54 (Start at last previous offset G56)
Tap: G54 G55 G56 (Start at last previous offset G54)

I would say no. I also do not believe there would be an easy way to sort the offsets for them to come out exactly like you would want either. I have seen some post processors (PostHaste) that will use dumb logic and simply reverse the order the offsets are called. That can save some time if you are running identical parts and using subroutines, but what happens if all 3 machine setups use the same center drill, same drill, but say the tap needs to be a bottoming tap on the G55 machine setup? Sorting what would be "faster" immediately gets very complex, very quickly.

If you need this kind of precise control, it must be done manually IMO.

**TonyW** · 09-04-2013, 06:26 PM

Only thing I can think of is to make more Machine setups. In this case there would be 6. 1st three forward order, 2nd three in reverse order, then 3rd in forward order again. Then all you have to do is save/load the features you already made and want to use to each new setup. I think that should work.

**pp-TG** · 09-04-2013, 06:26 PM

Originally Posted by SBC Cycle

I'm thinking he is looking for something like option 3 (by Tool) but instead of going:

Center Drill: G54 G55 G56
Drill: G54 G55 G56
Tap: G54 G55 G56

Center Drill: G54 G55 G56
Drill: G56 G55 G54 (Start at last previous offset G56)
Tap: G54 G55 G56 (Start at last previous offset G54)

I would say no. I also do not believe there would be an easy way to sort the offsets for them to come out exactly like you would want either. I have seen some post processors (PostHaste) that will use dumb logic and simply reverse the order the offsets are called. That can save some time if you are running identical parts and using subroutines, but what happens if all 3 machine setups use the same center drill, same drill, but say the tap needs to be a bottoming tap on the G55 machine setup? Sorting what would be "faster" immediately gets very complex, very quickly.

If you need this kind of precise control, it must be done manually IMO.

Yes, thanks, this is exactly what I was talking about. And not being possible was what I was afraid of

Hand editing is an option I guess but just don't like to, if it can be avoided but the way it post does add lots of time to a program. The other software I have will post them in the order they were picked or if you use last selected can be reversed. So no real work around other then hand editing? No way to make them post in order of selected?

And Al, I do have my post setup to force the workshifts at machine setups. But I do get kind of a funny thing I have not been able to figure out on posting. If I take all the info out of 16(machine setup change) so it is totally blank, don't like the clutter, it puts an M0 before changing workshifts? If I put a blank space on the next line right after the #16 and then the following line put a "" "" end of block it puts a space before the machine setup change instead of an M0. I can't for the life of me figure out where it is getting the M0 when left blank?

16. Machine Setup Change

16. Machine Setup Change

"" ""

The first one above gives me an M0 when posted the second just gives me a end of block before the change. Any idea where it is pulling the M0 from?

**pp-TG** · 09-04-2013, 06:33 PM

Originally Posted by TonyW

Only thing I can think of is to make more Machine setups. In this case there would be 6. 1st three forward order, 2nd three in reverse order, then 3rd in forward order again. Then all you have to do is save/load the features you already made and want to use to each new setup. I think that should work.

Hey Tony,

Little confused at this. Are you saying make a machine setup for each tool in each direction? So basically make one for the spot drill on G54 then another for G55 then another for G56 then on the 4th machine setup use this for the drill on G56 then another setup for G55 and so on? I have not tried this but pretty much everything else.

**jrmach** · 09-04-2013, 07:12 PM

The only way I can think of is a feature made for each offset/tool.
For example,,for a c-drill,drill,tap routine,with 3 offsets(54,55,56),,you would have to do a single feature such as c-drill,pick by order.That should do all 3 holes in order with different offsets.Now,you would have to do 3 different drill,each one the offset you want(56,55,54)in the order you want,,same for tap,3 different tap,each one withe offset you want(54,55,56).
Also under current setting/part,,post by feature.
A lot of work for sure,but if you are looking to shave seconds,,,,I take it you must be running hundreds or thousands of parts.

**jrmach** · 09-04-2013, 07:25 PM

Here is an example.I am not even using three machine set-ups,but am using 3 offsets.Just to show the work flow.Save/load feature makes quicker work of this for sure.
So the answer to your original question is No.At least not that I know of.But there are ways to get the desired result,if worth the time.

**TonyW** · 09-04-2013, 07:32 PM

1st three setups, spot drill (G54, G55, G56). 2nd 3, drill tap hole (G56,G55,G54), 3rd three, tap holes (G54,G55,G56). Pretty much like you said. You can right click features and save them. Then right click your new setup, and load the feature. Kind of like copy and paste

And the stop thing was making me nuts too. There is a thread here somewhere i just cant find it. Line 16 on my HAAS post looks like this:

16. Machine Setup Change
" "
n,"G91 G28 Z0"
n,"G91 G28 Y0"
n,stop
"(NEXT MACHINE SETUP - ",setup_name,")"
" "

That's to post stops. to stop the posting of stops, on Line 626 I set the stops to off, like this:

626. Stop? ""

**SBC Cycle** · 09-04-2013, 07:58 PM

None that I'm aware of other than breaking up all your features and manually changing each feature's Work Offset.

In similar circumstances, that meant (for me) a feature for every operation, every Work Offset change.

Feature Center Drill - G54
Feature Center Drill - G55
Feature Center Drill - G56

Feature Drill - G56
Feature Drill - G57
Feature Drill - G58

....so on so forth. One Machine Setup, posting by feature. There could be a better way but I have been bit too many times by letting the software pick the order of things for me. I have removed all compound operations every update/upgrade. Tap feature only taps, drill only drills. That's also how I can spot drill from right to left, drill from left to right, and tap from right to left. Maybe I'm just a control freak but that's how it's done here.

**jrmach** · 09-04-2013, 07:59 PM

Tony,try my file,,,,if I understand what you guys are getting with the M00,,you don't get that the way I did it.Making individual machine set-ups are not necessary at all for the example at hand.

**pp-TG** · 09-04-2013, 08:01 PM

Originally Posted by jrmach

Here is an example.I am not even using three machine set-ups,but am using 3 offsets.Just to show the work flow.Save/load feature makes quicker work of this for sure.
So the answer to your original question is No.At least not that I know of.But there are ways to get the desired result,if worth the time.

Yes this way does work and forgot to mention I have done it this way but this only works when using one machine setup and that is ok if you are programming from 2d geometry and can move everything to the same zero point and just use layers to separate everything but if programming from models this does not work because of the need for machine setups for additional zero points. (At least I have not got it to work with machine setups) It may be the best option I can see, it is just that one of my favorite options over my other software were being able to bring in the model and easily set multiple zeros and have the part fixture and everything brought in as an assembly.

Originally Posted by TonyW

1st three setups, spot drill (G54, G55, G56). 2nd 3, drill tap hole (G56,G55,G54), 3rd three, tap holes (G54,G55,G56). Pretty much like you said. You can right click features and save them. Then right click your new setup, and load the feature. Kind of like copy and paste

And the stop thing was making me nuts too. There is a thread here somewhere i just cant find it. Line 16 on my HAAS post looks like this:

16. Machine Setup Change
" "
n,"G91 G28 Z0"
n,"G91 G28 Y0"
n,stop
"(NEXT MACHINE SETUP - ",setup_name,")"
" "

That's to post stops. to stop the posting of stops, on Line 626 I set the stops to off, like this:

626. Stop? ""

Are you meaning setups or features? I have done this with multiple features and it works but not when I do multiple setups? (I still may be confused here

)

And yes not sure what the M0 is all about but you can leave on 626 if you want if you just put a blank line before your "" "" right after 16 Machine setup change and even without that and 626 it still puts in the space any way so I don't want all M0 capabilities disabled so this works ok other then the end of block in the program..... (Yes I am a bit OCD on my file format.....lol)

Thanks again for all the ideas guys it sure helps to have someone to bounce things off.

**pp-TG** · 09-04-2013, 08:11 PM

Originally Posted by SBC Cycle

None that I'm aware of other than breaking up all your features and manually changing each feature's Work Offset.

In similar circumstances, that meant (for me) a feature for every operation, every Work Offset change.

Feature Center Drill - G54
Feature Center Drill - G55
Feature Center Drill - G56

Feature Drill - G56
Feature Drill - G57
Feature Drill - G58

....so on so forth. One Machine Setup, posting by feature. There could be a better way but I have been bit too many times by letting the software pick the order of things for me. I have removed all compound operations every update/upgrade. Tap feature only taps, drill only drills. That's also how I can spot drill from right to left, drill from left to right, and tap from right to left. Maybe I'm just a control freak but that's how it's done here.

Yes I do the same thing. I like to pick center drill, drill, and tap by individual feature also. I have mine defaulted the same way. It is only an issue for multiple machine setups. If you only have one then it is not a big deal. But with solid models you really have no choice but to use multiple machine setups.

**pp-TG** · 09-04-2013, 08:13 PM

Originally Posted by jrmach

Tony,try my file,,,,if I understand what you guys are getting with the M00,,you don't get that the way I did it.Making individual machine set-ups are not necessary at all for the example at hand.

I agree but how do you work around programming solids? Or do you mostly use 2d geometry?

**jrmach** · 09-04-2013, 08:24 PM

Mostly 2D.It is all about the work we do.99 percent of my jobs are on napkins and a customer explaining what he wants,ha.Not only that,but usually only 1 or 2 parts.
But NOW,I see what you are talking about.Little different than original question.

JSYK,the one person most likely to figure stuff out,won't.Need to Un-Burn some bridges my friend.

**pp-TG** · 09-04-2013, 09:01 PM

Originally Posted by jrmach

Mostly 2D.It is all about the work we do.99 percent of my jobs are on napkins and a customer explaining what he wants,ha.Not only that,but usually only 1 or 2 parts.
But NOW,I see what you are talking about.Little different than original question.

JSYK,the one person most likely to figure stuff out,won't.Need to Un-Burn some bridges my friend.

Sorry for the confusion with the original question..... I guess it made sense to me

Thanks for the help. I guess it is nice to know I wasn't just overlooking something. It looks like it will either need to be done in 2d or cutting and pasting......

On a similar note is this the same way you guys deal with contouring? If I have lets say a 3/16" EM doing two counter bores on the same workshift and I want a rough pass and finish pass it will do both rough then back to the first and finish it then to the other and finish that. Individual features for rough and finish one hole at a time best way?

**jrmach** · 09-04-2013, 09:20 PM

Me ? ? What I do,is not necessarily best for someone else. Onesy,Twosy,,Faster I post code,faster I am done.So,I don't Optimize/or get Control Freakish.If I spend an extra 5-10 minutes programming,just to save 2 minutes,,it don't make sense.Also,I only use my CNC part of the time,even though the whole job could be done on it.If my manual machines can be faster for what is at hand,I use them.Faster the job is done,more I make.So to answer your question,it will depend on each job and how many parts,,just depends.

**pp-TG** · 09-04-2013, 09:52 PM

Understandable for that type of work. Thanks again.

**TonyW** · 09-04-2013, 09:55 PM

Ok JR, yeah, I see that. I do things that way sometimes too. Just wanted to throw out how to use machine setups to do different things. I guess your way is easier anyway

PP: Yeah, sometimes I want stops too. That's why I have multiple posts of the same machine. Each one does something a little different depending on my particular setup needs. Can always copy and paste the posts and name them something else

What I was told was that the stops are there for people who use one vise, but stop in between machine setups to rotate the part in vise, etc. Guess thats what its for. Usually I'm running my other post without the stops, and I have lots of optional stops in program so I can always stop where I want when I have it active in controller.

And I meant multiple machine setups. Only problem I forgot to mention is when you load a saved feature into the setup, it does not automatically switch to the setups offset number. Still have to edit the feature and change the offset. Sorry 'bout that.

**pp-TG** · 09-04-2013, 10:20 PM

Thanks for the clarification Tony. I have not tried this yet so I will see if I can get that to work.

Thread: Machining order

Thread Tools

Search Thread

Display

Machining order

Similar Threads

05 How to order by layer

Cut order?

New IH on order...

V23 machining order change?

New VF-5 on order

Posting Permissions

My IndustryArena Login

My IndustryArena Login

Thread: Machining order

Machining order

Similar Threads

Posting Permissions

This website uses cookies