Transform Toolpath

[Rekd™]

I don't use this much, but when I do, I generally get screwed one way or another.

 

I have a part with 2 operations at G54 and G55, using WCS to create the planes and assign the WFO's. I'm running a 2 vise setup, top and bottom at G54 & G55 respectively. Life is good.

 

Now I want to add 2 more vises, G56 & G57. So I copied my WCS's and assigned new WFO's to them, because Edit Common Parameters STILL DOESN'T WORK. Now I select Between Views as the translation method, select the new view as the destination, and it doesn't accept the new WFO's.

 

WTF is up with WCS and WFO and translate between views?

 

Is it my post?

 

Is it me?

 

I really don't want to create all new ops, then have to manually go thru and change 58 freakin' operations at 12 clicks per operation!!

 

'Rekd teh Stupid Computors!

[crazy^millman]

Doing the same freaking thing right now Rekd as we speak.

 

 

Crazy is going to try tranform and tell it to create operation for him then just edit the toolpane page if it works.

 

Crazy Millman

[crazy^millman]

Well Rekd it worked if I did create new geomentry and operation but since I am using soilds for a control it wouldn't for those operations. Then of course it sucks cause I need to do for 4 vicea and doesn't do it order so will have to do it in groups I guess.

 

 

Crazy Millman

 

What I have done in the past is create groups using just one tool for all operation for that tool and then do all operation for that group then close it and then go that way. It sure beat the old cut and paste. I may be like you I dont trust the posted program without geomentry to drive it all for all vices. (sorry Rekd I meant operation not geomentry)

 

[ 10-25-2003, 02:42 PM: Message edited by: Millman^Crazy ]

[Rekd™]

I've always had problems with this. That's why I use my own program to generate sub programs on the NC files. Only problem is, it's designed to only work on files with only a single offset (G54 OR G55, not AND G55) in it.

 

There's got to be an easier way. I'm NOT gonna create new ops, new geometry and tripple the file sizes...

 

'Rekd

 

[ 10-25-2003, 02:44 PM: Message edited by: Rekd ]

[crazy^millman]

Yeah is does suck but since I dont have the tools you have I am kinda stuck doing it this way. I could cut and paste a g-gode program but why the F do that. I have had it do good with using sub on transform but dont really like the sub program rotue that is why I am tryign to get my sub routine MpMaster post workign then it keeps it all in one program of course the dwon side is it has to be smaller that 4 mb to use it. Another reason I have worked out the L9000 cycels for the post I can do alot of the 2d pockets with one line of code that way and save a ton of space in the program to acheive my subroutine process.

 

 

Crazy Millman

[Rekd™]

Several years ago I made an app in VB that reads the NC files and breaks them up by tool number, then recombines them as sub programs.

 

Here's a before and after

 

Before M98 Px:

 

code:

---

%

O0001

(M98PX SAMPLE.NCF)

(OCT 25, 2003 12:00)

(MACHINE: 3 AXIS)

(MATERIAL: ALUMINUM INCH - 6061)

(STOCK SIZE: X 4.75 Y 5. Z 1.5)

(TOOL 1: DIA 3.0000 3" Face Mill)

(TOOL 4: DIA 0.2500 1/4 CHAMFER MILL)

(TOOL 5: DIA 0.0938 3/32 DRILL)

(TOOL 6: DIA 0.1100 #35 DRILL)

(OVERALL MAX Z1.)

(OVERALL MIN Z-.3982)

N1 G00 G17 G40 G49 G80 G90 G20

N2 M01

( OPERATION: 1 FACING )

N3 ( OP 1 G54 )

N4 ( FACE )

N5 T1 M06(T1: 3" FACE MILL)

N6 M03 S3500

N7 G00 G90 G54 X-.001 Y-6.875

N8 G43 H1 Z1. M08

N9 Z.11

N10 G01 Z0. F50.

N11 Y.45 F75.

N12 G03 X-2.3125 I-1.1558 J0.

N13 G01 Y-5.075

N14 G02 X-4.624 I-1.1558 J0.

N15 G01 Y2.25

N16 G00 Z1.

N17 M09

N18 G90

N19 M01

( OPERATION: 2 DRILL )

N20 ( OP 1 G54 )

N21 ( SPOT 2-56 HELICOIL THRU )

N22 T4 M06(T4: 1/4 CHAMFER MILL)

(MAX-DEPTH | Z-.056)

N23 M03 S7000

N24 G00 G90 G54 X-3.862 Y-.775

N25 G43 H4 Z1. M08

N26 G99 G82 X-3.862 Y-.775 Z-.043 R.1 P.3 F25.

N27 X-4.187 Y-2.9 P.3

N28 X-2.187 Y-.85 P.3

N29 X-1.107 Y-2.862 P.3

N30 Y-2.05 P.3

N31 Y-.887 P.3

N32 G80

(OPERATION: 3 DRILL)

N33(OP 1 G54)

N34(SPOT .110)

(T4: 1/4 CHAMFER MILL)

N35 X-.575 Y-2.472

N36 G99 G82 X-.575 Y-2.472 Z-.056 R.1 P.3 F25.

N37 Y-2.047 P.3

N38 Y-1.737 P.3

N39 X-.425 Y-1.157 P.3

N40 G80

N41 M09

N42 G90

N43 M01

( OPERATION: 4 DRILL )

N44 ( OP 1 G54 )

N45 ( DRILL 2-56 HELICOIL THRU )

N46 T5 M06(T5: 3/32 DRILL)

(MAX-DEPTH | Z-.3982)

N47 M03 S7000

N48 G00 G90 G54 X-3.862 Y-.775

N49 G43 H5 Z1. M08

N50 G99 G83 X-3.862 Y-.775 Z-.3982 R.1 I.1875 J.0469 K.0469 F12.

N51 X-4.187 Y-2.9

N52 X-2.187 Y-.85

N53 X-1.107 Y-2.862

N54 Y-2.05

N55 Y-.887

N56 G80

N57 M09

N58 G90

N59 M01

( OPERATION: 5 DRILL )

N60 ( OP 1 G54 )

N61 ( DRILL .110 )

N62 T6 M06(T6: #35 DRILL)

(MAX-DEPTH | Z-.203)

N63 M03 S7000

N64 G00 G90 G54 X-.575 Y-2.472

N65 G43 H6 Z1. M08

N66 G99 G83 X-.575 Y-2.472 Z-.203 R.1 I.22 J.055 K.055 F15.

N67 Y-2.047

N68 Y-1.737

N69 X-.425 Y-1.157

N70 G80

N71 M09

N72 G91 G28 Z0.

N73 G91 G28 Y0.

N74 G90

N75 T1 M06

N76 M30

%

---

After

 

code:

---

%

O0001

(M98PX SAMPLE.NCF)

(OCT 25, 2003 12:00)

(MACHINE: 3 AXIS)

(MATERIAL: ALUMINUM INCH - 6061)

(STOCK SIZE: X 4.75 Y 5. Z 1.5)

(TOOL 1: DIA 3.0000 3" Face Mill)

(TOOL 4: DIA 0.2500 1/4 CHAMFER MILL)

(TOOL 5: DIA 0.0938 3/32 DRILL)

(TOOL 6: DIA 0.1100 #35 DRILL)

(OVERALL MAX Z1.)

(OVERALL MIN Z-.3982)

N1 G00 G17 G40 G49 G80 G90 G20

N2 M01

( OPERATION: 1 FACING )

N3 ( OP 1 G54 )

N4 ( FACE )

N5 T1 M06(T1: 3" FACE MILL)

N6 M03 S3500

N7 G00 G90 G54 X-.001 Y-6.875

N8 G43 H1 Z1. M08

G54 G17 X-.001 Y-6.875

M98 P3

/ G55 G17 X-.001 Y-6.875

/ M98 P3

/ G56 G17 X-.001 Y-6.875

/ M98 P3

/ G57 G17 X-.001 Y-6.875

/ M98 P3

N17 M09

N18 G90

N19 M01

( OPERATION: 2 DRILL )

N20 ( OP 1 G54 )

N21 ( SPOT 2-56 HELICOIL THRU )

N22 T4 M06(T4: 1/4 CHAMFER MILL)

(MAX-DEPTH | Z-.056)

N23 M03 S7000

N24 G00 G90 G54 X-3.862 Y-.775

N25 G43 H4 Z1. M08

G54 G17 X-3.862 Y-.775

M98 P4

/ G55 G17 X-3.862 Y-.775

/ M98 P4

/ G56 G17 X-3.862 Y-.775

/ M98 P4

/ G57 G17 X-3.862 Y-.775

/ M98 P4

N41 M09

N42 G90

N43 M01

( OPERATION: 4 DRILL )

N44 ( OP 1 G54 )

N45 ( DRILL 2-56 HELICOIL THRU )

N46 T5 M06(T5: 3/32 DRILL)

(MAX-DEPTH | Z-.3982)

N47 M03 S7000

N48 G00 G90 G54 X-3.862 Y-.775

N49 G43 H5 Z1. M08

G54 G17 X-3.862 Y-.775

M98 P5

/ G55 G17 X-3.862 Y-.775

/ M98 P5

/ G56 G17 X-3.862 Y-.775

/ M98 P5

/ G57 G17 X-3.862 Y-.775

/ M98 P5

N57 M09

N58 G90

N59 M01

( OPERATION: 5 DRILL )

N60 ( OP 1 G54 )

N61 ( DRILL .110 )

N62 T6 M06(T6: #35 DRILL)

(MAX-DEPTH | Z-.203)

N63 M03 S7000

N64 G00 G90 G54 X-.575 Y-2.472

N65 G43 H6 Z1. M08

G54 G17 X-.575 Y-2.472

M98 P6

/ G55 G17 X-.575 Y-2.472

/ M98 P6

/ G56 G17 X-.575 Y-2.472

/ M98 P6

/ G57 G17 X-.575 Y-2.472

/ M98 P6

N71 M09

N72 G91 G28 Z0.

N73 G91 G28 Y0.

N74 G90

N75 T1 M06

N76 M30

O3 ( SUB NUMBER: 3 )

N9 Z.11

N10 G01 Z0. F50.

N11 Y.45 F75.

N12 G03 X-2.3125 I-1.1558 J0.

N13 G01 Y-5.075

N14 G02 X-4.624 I-1.1558 J0.

N15 G01 Y2.25

N16 G00 Z1.

M99

O4 ( SUB NUMBER: 4 )

N26 G99 G82 X-3.862 Y-.775 Z-.043 R.1 P.3 F25.

N27 X-4.187 Y-2.9 P.3

N28 X-2.187 Y-.85 P.3

N29 X-1.107 Y-2.862 P.3

N30 Y-2.05 P.3

N31 Y-.887 P.3

N32 G80

(OPERATION: 3 DRILL)

N33(OP 1 G54)

N34(SPOT .110)

(T4: 1/4 CHAMFER MILL)

N35 X-.575 Y-2.472

N36 G99 G82 X-.575 Y-2.472 Z-.056 R.1 P.3 F25.

N37 Y-2.047 P.3

N38 Y-1.737 P.3

N39 X-.425 Y-1.157 P.3

N40 G80

M99

O5 ( SUB NUMBER: 5 )

N50 G99 G83 X-3.862 Y-.775 Z-.3982 R.1 I.1875 J.0469 K.0469 F12.

N51 X-4.187 Y-2.9

N52 X-2.187 Y-.85

N53 X-1.107 Y-2.862

N54 Y-2.05

N55 Y-.887

N56 G80

M99

O6 ( SUB NUMBER: 6 )

N66 G99 G83 X-.575 Y-2.472 Z-.203 R.1 I.22 J.055 K.055 F15.

N67 Y-2.047

N68 Y-1.737

N69 X-.425 Y-1.157

N70 G80

M99

%

( File Size: 2.6kb )

( File Length: 139 lines )

( File Modified 10/25/2003 at 12:01:40 PM )

---

This works great for proofed NC files also. The processing time to manually create this file would be around 5 to 10 minutes, depending on the person. The time to process it with my program is roughly .15 seconds. (Can be as much as 3 to 5 seconds on a 1 meg file, and we won't discuss how long it would take to do THAT manually.. )

 

Here's the interface..

 

 

'Rekd

[crazy^millman]

You sell copies of the little utility where. That is freaking cool Rekd. I am doign that very exact thing I do one complete proff it all out then I just cpoy the ops for each fixture offset which made it 72 ops long on this easy one and go from there. Thnat looks real good Rekd. Teh make Millman see the need for VB.

 

Crazy Millman

[Rekd™]

I've refrained from marketing it yet because there's just too many different types of code out there. This is geared to Fanucs, and works very well with them.

 

Now with Mastercam supporting subs much better than they used to, there's not going to be as much of a market for it.

 

'Rekd teh day late and a byte short

[Müřlıń®]

I wish I was half as smart as you two on this VB stuff

 

 

Murlin teh VB retarded.....

 

[ 10-25-2003, 06:08 PM: Message edited by: Murlin ]

[crazy^millman]

Us 2 Murlin well I don't think Rekd's got a mouse in his pocket. I am as dumb as they come to VB. I want to learn it but unless soemoen is going to give me the devoplers kit or buy it for me that si a long ways off.

 

 

Crazy Millman

[Rekd™]

Millman, do you have MS Office? If so you've got a somewhat stripped down version of it already. You can't make an executable, but you can create forms, use objects, access the system, lots of things to learn the program structs and syntax.

 

'Rekd

[crazy^millman]

Yep sure do Rekd if you want to I would appericate that tredmonusly. Shoot it to my email and I will take a look but if it is an .exe ending outlook has a moo cow to may have to zip it for me to get it. I am going to zip up some things for you to see.

 

 

Crazy Millman

[crazy^millman]

Here is what I can get transform to do Matt. I just don't trust it yet to do what I want for 6 and 8 hour run times if you catch my drift.

 

code:

---

%

O9999 (T)

(MC9 FILE - C:MCAM91MILLMC9CIRMILLPECK.MC9)

(PROGRAM LOCATION - C:MCAM91MILLNCT.NC)

(DATE - OCT-25-03)

(TIME - 19:02)

(T10 | 1/4 FLAT ENDMILL | H10 | D10 | D0.2500" | | CONTOUR....)

(T11 | 1/8 FLAT ENDMILL | H11 | D11 | D0.1250" | | CONTOUR....)

(OVERALL MAX | Z.25)

(OVERALL MIN | Z-.05)

G0G17G40G80G90

T10M6( 1/4 FLAT ENDMILL)

(MAX | Z.25)

(MIN | Z-.05)

G0G90E1X-3.0041Y2.0752S5000M3

H10Z.25M8

G4 P2000

G8

M98P0001L1

G0E2X-3.0041Y2.0752Z.25

M98P0002L1

G0E3X-3.0041Y2.0752Z.25

M98P0003L1

G0E4X-3.0041Y2.0752Z.25

M98P0004L1

G91G28Z0.

M1

T11M6( 1/8 FLAT ENDMILL)

(MAX | Z.25)

(MIN | Z-.05)

G0G90E1X-1.523Y.569S4278M3

H11Z.25

G4 P2000

G8

M98P0005L1

G0E2X-1.523Y.569Z.25

M98P0006L1

G0E3X-1.523Y.569Z.25

M98P0007L1

G0E4X-1.523Y.569Z.25

M98P0008L1

G91G28Z0.

(MCUSTOCK X0. Y0. Z0. OTC OX0. OY0. OZ0.)

(MCUPTOOL T10 D0.25 L3. F3.)

M02

 

O0001

M8

Z.1

G1Z-.05F5.

G3Y2.1752I0.J.05F20.

Y1.9752I0.J-.1

Y2.1752I0.J.1

Y2.0752I0.J-.05

G0Z.25

M99

 

O0002

Z.1

G1Z-.05F5.

G3Y2.1752I0.J.05F20.

Y1.9752I0.J-.1

Y2.1752I0.J.1

Y2.0752I0.J-.05

G0Z.25

M99

 

O0003

Z.1

G1Z-.05F5.

G3Y2.1752I0.J.05F20.

Y1.9752I0.J-.1

Y2.1752I0.J.1

Y2.0752I0.J-.05

G0Z.25

M99

 

O0004

Z.1

G1Z-.05F5.

G3Y2.1752I0.J.05F20.

Y1.9752I0.J-.1

Y2.1752I0.J.1

Y2.0752I0.J-.05

G0Z.25

M99

 

O0005

Z.1

G1Z-.05F6.16

G3Y.7315I0.J.0813

Y.4065I0.J-.1625

Y.7315I0.J.1625

Y.569I0.J-.0813

G0Z.25

M99

 

O0006

Z.1

G1Z-.05F6.16

G3Y.7315I0.J.0813

Y.4065I0.J-.1625

Y.7315I0.J.1625

Y.569I0.J-.0813

G0Z.25

M99

 

O0007

Z.1

G1Z-.05F6.16

G3Y.7315I0.J.0813

Y.4065I0.J-.1625

Y.7315I0.J.1625

Y.569I0.J-.0813

G0Z.25

M99

 

O0008

Z.1

G1Z-.05F6.16

G3Y.7315I0.J.0813

Y.4065I0.J-.1625

Y.7315I0.J.1625

Y.569I0.J-.0813

G0Z.25

M99

%

---

It looks close to what you got but done all with the Transform. I dont like the fact it feels the need to write 4 different subs when it only needs one. I like this but you have to do this for all the tools used. I guess I could do a sort of tools from that if I created the operation but still real weary of doing it this way. I have no problem looping and cutting G-Code and use that just worry that it is going to add or something like that if doing the Transform thing.

 

Crazy Millman

 

[ 10-25-2003, 10:08 PM: Message edited by: Millman^Crazy ]

[crazy^millman]

code:

---

 %

O0000 (T)

(MC9 FILE - C:MCAM91MILLMC9CIRMILLPECK.MC9)

(PROGRAM LOCATION - C:MCAM91MILLNCT.NC)

(DATE - OCT-25-03)

(TIME - 19:20)

(T10 | 1/4 FLAT ENDMILL | H10 | D10 | D0.2500" | | CONTOUR....)

(T11 | 1/8 FLAT ENDMILL | H11 | D0 | D0.1250" | | CONTOUR....)

(OVERALL MAX | Z.25)

(OVERALL MIN | Z-.05)

G0G17G40G80G90

T10M6( 1/4 FLAT ENDMILL)

(MAX | Z.25)

(MIN | Z-.05)

G0G90X-3.0041Y2.0752S5000M3

H10Z.25M8

G4 P2000

G8

M98P0001L1

G91G28Z0.

M1

T11M6( 1/8 FLAT ENDMILL)

(MAX | Z.25)

(MIN | Z-.05)

G0G90X-1.523Y.569S4278M3

H11Z.25

G4 P2000

G8

M98P0002L1

G91G28Z0.

M02

 

O0001

Z.1

G1Z-.05F5.

G3Y2.1752I0.J.05F20.

Y1.9752I0.J-.1

Y2.1752I0.J.1

Y2.0752I0.J-.05

G0Z.25

M99

 

O0002

Z.1

G1Z-.05F6.16

G3Y.7315I0.J.0813

Y.4065I0.J-.1625

Y.7315I0.J.1625

Y.569I0.J-.0813

G0Z.25

M99

%

---

Here is what the above looks like when you do it as Group NCI by Operation Order checked it is clean now. It just does not do the multi offsets this way. If I get this to work with mulit offsets and then subroutines and keep it all in one program think I got it licked for as many vices as I want.

 

Crazy Millman

 

[ 10-26-2003, 11:15 PM: Message edited by: Millman^Crazy ]

[heeler]

Rekd,

 

I don't understand what you want to do, but we use tranform toolpath all the time with virtually (need spell checker on forum) no problems. If you can email me you file/or call me maybe I could help.

 

Glenn

 

P.S We don't use the WCS. Just tool plane/ construction plane.

[crazy^millman]

Heeler why is the codes I posted up so didferent when I all I changed was Group NCI by Operation Order then it doesn't output the workoffsets. Rekd has a way to do what he want but he want Mastercam to do it completely using the Transfrom and he I am bettign he is gettign the same results as me.

 

Crazy Millman

[heeler]

Crazy,

 

Because I havn't been able to get the WCS to work the way I want I'm not really sure that I can help you. But if you would like to email me a sample file, I can do it the way that we do and see if it would work for you. We use Workpiece offsets, subs and multiple parts. I'll certainly help with anything I can.

 

Glenn

[crazy^millman]

Yeah Heeler I dont use the WCS at all for 3 axis stuff I just move my models to the origin. I do use it for 4th axis stuff but only if I have too. I appericate the offer and will find soemthign for you to play with but I have tried every button and way on that transform and it just dosen't get it the way I like. I find it better to cut and paste change the workoffsets for each op effected and go from there. Beside anything over 4mb has to be dnc around here and you cant DNC subs very well.

 

Crazy Millman

[Craig-B]

We use transform operations with a modified Mpmaster and get this type of output for subprograms. It just depends on the transform parameter settings.

 

 

%

O7520 (BLOCK.CNC)

G0G17G20G40G49G80G90

N1T1( 1/8 CENTERDRILL)

M6

G0G90G54M8

G0G90G54X-1.75Y1.75S3000M3T2

G43H1Z2.

M98P0001

G0G90G55X-1.75Y1.75

Z2.

M98P0001

G0G90G56X-1.75Y1.75

Z2.

M98P0001

G0G90G57X-1.75Y1.75

Z2.

M98P0001

M5

G0G91G28Z0.M9

M01

 

N2T2( #72 DRILL)

M6

G0G90G54M8

G0G90G54X-1.75Y1.75S5000M3T3

G43H2Z2.

M98P0002

G0G90G55X-1.75Y1.75

Z2.

M98P0002

G0G90G56X-1.75Y1.75

Z2.

M98P0002

G0G90G57X-1.75Y1.75

Z2.

M98P0002

M5

G0G91G28Z0.M9

M01

 

N3T3( 1/4 FLAT ENDMILL)

M6

G0G90G54M8

G0G90G54X-.15Y-1.625S1069M3T1

G43H3Z2.

M98P0003

G0G90G55X-.15Y-1.625

Z2.

M98P0003

G0G90G56X-.15Y-1.625

Z2.

M98P0003

G0G90G57X-.15Y-1.625

Z2.

M98P0003

M5

G0G91G28Z0.M9

M11

G0G91G28Y0.

M10

M30

 

O0001(TOOL # 1 CINTERDRILL)

Z.1

G99G81Z-.2R.1F10.

X1.75

Y-1.75

X-1.75

G80

Z2.

M99

 

O0002(TOOL # 2 DRILL)

Z.1

G99G81Z-1.05R.1F3.42

X1.75

Y-1.75

X-1.75

G80

Z2.

M99

 

O0003(TOOL # 3 END MILL)

Z.1

G1Z0.10.

G42D3X0.

X.5Z-.0056

G3X1.625Y-.5Z-.0256I0.J1.125

G1Y.5Z-.0369

G3X.5Y1.625Z-.0569I-1.125J0.

G1X-.5Z-.0681

G3X-1.625Y.5Z-.0881I0.J-1.125

G1Y-.5Z-.0994

G3X-.5Y-1.625Z-.1194I1.125J0.

G1X0.Z-.125

X.5Z-.1306

G3X1.625Y-.5Z-.1506I0.J1.125

G1Y.5Z-.1619

G3X.5Y1.625Z-.1819I-1.125J0.

G1X-.5Z-.1931

G3X-1.625Y.5Z-.2131I0.J-1.125

G1Y-.5Z-.2244

G3X-.5Y-1.625Z-.2444I1.125J0.

G1X0.Z-.25

X.5Z-.2556

G3X1.625Y-.5Z-.2756I0.J1.125

G1Y.5Z-.2869

G3X.5Y1.625Z-.3069I-1.125J0.

G1X-.5Z-.3181

G3X-1.625Y.5Z-.3381I0.J-1.125

G1Y-.5Z-.3494

G3X-.5Y-1.625Z-.3694I1.125J0.

G1X0.Z-.375

X.5Z-.3806

G3X1.625Y-.5Z-.4006I0.J1.125

G1Y.5Z-.4119

G3X.5Y1.625Z-.4319I-1.125J0.

G1X-.5Z-.4431

G3X-1.625Y.5Z-.4631I0.J-1.125

G1Y-.5Z-.4744

G3X-.5Y-1.625Z-.4944I1.125J0.

G1X0.Z-.5

X.5

G3X1.625Y-.5I0.J1.125

G1Y.5

G3X.5Y1.625I-1.125J0.

G1X-.5

G3X-1.625Y.5I0.J-1.125

G1Y-.5

G3X-.5Y-1.625I1.125J0.

G1X0.

G40X.15

G0Z2.

M99

%

[Jack K]

We do multiple setups all the time. I like to use the old NCI edit the best you can change your wcs in one click as well as transform or mirror, ect..... you can also use toolpath transferin the operations manager as well.

 

 

Tool paths Transform

 

1. Translate = Tool plane origin only

2. Method = Tool plane

3. Group NCI output by = operation type

4. Copy source operation

5. Disable posting in selected operation

6. Work offset numbering = assign new set= 1 & 1

 

Translate

 

1. X = 0

2. Y =0

3. Number of steps in X..Set to # of vises (translates)

 

works good for me

[crazy^millman]

Ok guys well I wil try it again got the second side of the parts doing 4 at a time so it will be a good test I am also using a mpmaster modifed for the Fadal so I will see and go from there appeircate it.

 

 

Crazy Millman

[crazy^millman]

Well I humbly say thank you Jack work like a freaking champ that way. Here is the code I got and it worked with or without subs:

code:

---

%

O0900 (T)

(MC9 FILE - C:MCAM91MILLMC9OCTOGON PART.MC9)

(PROGRAM LOCATION - C:MCAM91MILLNCT.NC)

(DATE - OCT-27-03)

(TIME - 20:07)

(T1 | 1/8 CENTERDRILL | H0 | D0 | D0.1250" | | PECK DRILL.)

(T207 | 1/2-13 TAPRH | H0 | D0 | D0.5000" | | TAP........)

(OVERALL MAX | Z6.)

(OVERALL MIN | Z1.)

G0G17G40G80G90

T1M6( 1/8 CENTERDRILL)

(MAX | Z6.)

(MIN | Z2.75)

G0G90E1X0.Y0.S2139M3

H1Z6.M8

G4 P2000

G8

M98P0901L1

G0E2X0.Y0.Z6.

M98P0901L1

G0E3X0.Y0.Z6.

M98P0901L1

G0E4X0.Y0.Z6.

M98P0901L1

G0E5X0.Y0.Z6.

M98P0901L1

G91G28Z0.

M1

T207M6( 1/2-13 TAPRH)

(MAX | Z6.)

(MIN | Z1.)

G0G90E1X0.Y0.S534M3

S534.2M5

G84.2

H207Z6.M8

G4 P2000

G8

M98P0902L1

G0E2X0.Y0.Z6.

M98P0902L1

G0E3X0.Y0.Z6.

M98P0902L1

G0E4X0.Y0.Z6.

M98P0902L1

G0E5X0.Y0.Z6.

M98P0902L1

G91G28Z0.

M02

 

O0901

G83G98X0.Y0.Z2.75R03.1Q.1F1.03

X0.Y2.4

X0.Y4.8

X0.Y7.2

X0.Y9.6

X0.Y12.

G80

M99

 

O0902

G84.1G98X0.Y0.Z1.R03.1F534.2Q.0769

X0.Y2.4F41.14

X0.Y4.8

X0.Y7.2

X0.Y9.6

X0.Y12.

G80

M99

%

---

Without subs.

code:

---

%

O0900 (T)

(MC9 FILE - C:MCAM91MILLMC9OCTOGON PART.MC9)

(PROGRAM LOCATION - C:MCAM91MILLNCT.NC)

(DATE - OCT-27-03)

(TIME - 20:10)

(T1 | 1/8 CENTERDRILL | H0 | D0 | D0.1250" | | PECK DRILL.)

(T207 | 1/2-13 TAPRH | H0 | D0 | D0.5000" | | TAP........)

(OVERALL MAX | Z6.)

(OVERALL MIN | Z1.)

G0G17G40G80G90

T1M6( 1/8 CENTERDRILL)

(MAX | Z6.)

(MIN | Z2.75)

G0G90E1X0.Y0.S2139M3

H1Z6.M8

G4 P2000

G8

G83G98X0.Y0.Z2.75R03.1Q.1F1.03

X0.Y2.4

X0.Y4.8

X0.Y7.2

X0.Y9.6

X0.Y12.

G80

G0E2X0.Y0.Z6.

G83G98X0.Y0.Z2.75R03.1Q.1F1.03

X0.Y2.4

X0.Y4.8

X0.Y7.2

X0.Y9.6

X0.Y12.

G80

G0E3X0.Y0.Z6.

G83G98X0.Y0.Z2.75R03.1Q.1F1.03

X0.Y2.4

X0.Y4.8

X0.Y7.2

X0.Y9.6

X0.Y12.

G80

G0E4X0.Y0.Z6.

G83G98X0.Y0.Z2.75R03.1Q.1F1.03

X0.Y2.4

X0.Y4.8

X0.Y7.2

X0.Y9.6

X0.Y12.

G80

G0E5X0.Y0.Z6.

G83G98X0.Y0.Z2.75R03.1Q.1F1.03

X0.Y2.4

X0.Y4.8

X0.Y7.2

X0.Y9.6

X0.Y12.

G80

G91G28Z0.

M1

T207M6( 1/2-13 TAPRH)

(MAX | Z6.)

(MIN | Z1.)

G0G90E1X0.Y0.S534M3

S534.2M5

G84.2

H207Z6.M8

G4 P2000

G8

G84.1G98X0.Y0.Z1.R03.1F534.2Q.0769

X0.Y2.4F41.14

X0.Y4.8

X0.Y7.2

X0.Y9.6

X0.Y12.

G80

G0E2X0.Y0.Z6.

G84.1G98X0.Y0.Z1.R03.1F534.2Q.0769

X0.Y2.4F41.14

X0.Y4.8

X0.Y7.2

X0.Y9.6

X0.Y12.

G80

G0E3X0.Y0.Z6.

G84.1G98X0.Y0.Z1.R03.1F534.2Q.0769

X0.Y2.4F41.14

X0.Y4.8

X0.Y7.2

X0.Y9.6

X0.Y12.

G80

G0E4X0.Y0.Z6.

G84.1G98X0.Y0.Z1.R03.1F534.2Q.0769

X0.Y2.4F41.14

X0.Y4.8

X0.Y7.2

X0.Y9.6

X0.Y12.

G80

G0E5X0.Y0.Z6.

G84.1G98X0.Y0.Z1.R03.1F534.2Q.0769

X0.Y2.4F41.14

X0.Y4.8

X0.Y7.2

X0.Y9.6

X0.Y12.

G80

G91G28Z0.

M02

%

---

Thanks and I hope they let me stick around glad to learn soemthing from others.

 

Crazy Millman

[crazy^millman]

Ok I ma freaking stumped on this one and been here 13 hours smelling smoke and crap and I am losign my patience. I did this at home worked peferect I try it here at work doesn't work. I have checked recheck and tripe checked I had the operator soem in here and see I have it the same way and I have tried it every freakign way wit heverything on to off will not post out the freaking offsets now.

 

Crazy Millman

[crazy^millman]

Well I freaking fixed it so simple of a thing I dont know why I just do have my computer do ti automatically. I just truned the freaking thing off and truned it back on put everything back to the origainl way it worked perfect.

 

Crazy thinks the smoke is making his computer sick as him.

[Rekd™]

LoL!

 

'Rekd