Posting for multiple vises

[jorges]

I programmed a prototype part a few months ago (X2 MR2) now is going on production.

I have to make a few hundreds now and I'd like to run 3 vises (a part per vise).

Is there a way to post my original program for 3 vises giving each vise a different work offset.

I tried trasform-translate but could not figured it out the work offset part.

Any help please

Thanks

[crazy^millman]

Yes Transform using toolplane. Make sure you increment work offset, and should be good. I made you an example file and put it in the X2 folder called CRAZY_TRANSFORM_3VICES.MCX Also make sure you check the toolplane only origin button as well.

 

Here is sample code from that:

code:

---

%

O0000 (T)

(MACHINE - MIGHTY/YAMA SEIKI)

(CUSTOMER - ADD CUSTOMER)

(PART # - Machine Group-2)

(MODEL # - Machine Group-2.MCX)

(PROGRAMMER - RON

(PROGRAM NAME - T.NC)

(DATE - APR-15-2008)

(TIME - 1:52 PM)

(PROGRAM REV - N/C)

(T10 - 1/2 INCH FLAT ENDMILL - H10 - D10 - D0.5000")

(T1 - 1/8 CENTERDRILL - H1 - D0.1250")

(T91 - 1/8 DRILL - H91 - D0.1250")

(OVERALL MAX - Z.25)

(OVERALL MIN - Z-.25)

N100 G0 G17 G20 G40 G80 G90

N110 T10 M06 (1/2 INCH FLAT ENDMILL)

N120 (MAX - Z.25)

N130 (MIN - Z-.25)

N140 G0 G54 X-1.25 Y-1. S1069 M3

N150 G43 H10 Z.25

N160 Z.1

N170 G94 G1 Z-.25 F6.42

N180 X-.75

N190 G3 X-.25 Y-.5 I0. J.5

N200 G1 Y0.

N210 G2 X0. Y.25 I.25 J0.

N220 G1 X1.

N230 G2 X1.25 Y0. I0. J-.25

N240 G1 Y-1.

N250 G2 X1. Y-1.25 I-.25 J0.

N260 G1 X0.

N270 G2 X-.25 Y-1. I0. J.25

N280 G1 Y-.5

N290 G3 X-.75 Y0. I-.5 J0.

N300 G1 X-1.25

N310 Z-.15 F25.

N320 G0 Z.25

N330 G55 X-1.25 Y-1. Z.25

N340 Z.1

N350 G1 Z-.25 F6.42

N360 X-.75

N370 G3 X-.25 Y-.5 I0. J.5

N380 G1 Y0.

N390 G2 X0. Y.25 I.25 J0.

N400 G1 X1.

N410 G2 X1.25 Y0. I0. J-.25

N420 G1 Y-1.

N430 G2 X1. Y-1.25 I-.25 J0.

N440 G1 X0.

N450 G2 X-.25 Y-1. I0. J.25

N460 G1 Y-.5

N470 G3 X-.75 Y0. I-.5 J0.

N480 G1 X-1.25

N490 Z-.15 F25.

N500 G0 Z.25

N510 G56 X-1.25 Y-1. Z.25

N520 Z.1

N530 G1 Z-.25 F6.42

N540 X-.75

N550 G3 X-.25 Y-.5 I0. J.5

N560 G1 Y0.

N570 G2 X0. Y.25 I.25 J0.

N580 G1 X1.

N590 G2 X1.25 Y0. I0. J-.25

N600 G1 Y-1.

N610 G2 X1. Y-1.25 I-.25 J0.

N620 G1 X0.

N630 G2 X-.25 Y-1. I0. J.25

N640 G1 Y-.5

N650 G3 X-.75 Y0. I-.5 J0.

N660 G1 X-1.25

N670 Z-.15 F25.

N680 G0 Z.25

N690 M5

N700 G91 G28 Z0.

N710 M01

N720 T1 M06 ( 1/8 CENTERDRILL)

N730 (MAX - Z.1)

N740 (MIN - Z-.1)

N750 G0 G90 G54 X.25 Y-.25 S2139 M3

N760 G43 H1 Z.1

N770 G99 G81 Z-.1 R.1 F1.03

N780 X.75

N790 X.25 Y-.75

N800 X.75

N810 X.5 Y-.5

N820 G80

N830 G55 X.25 Y-.25 Z.1

N840 G99 G81 Z-.1 R.1 F1.03

N850 X.75

N860 X.25 Y-.75

N870 X.75

N880 X.5 Y-.5

N890 G80

N900 G56 X.25 Y-.25 Z.1

N910 G99 G81 Z-.1 R.1 F1.03

N920 X.75

N930 X.25 Y-.75

N940 X.75

N950 X.5 Y-.5

N960 G80

N970 M5

N980 G91 G28 Z0.

N990 M01

N1000 T91 M06 ( 1/8 DRILL)

N1010 (MAX - Z.1)

N1020 (MIN - Z-.1)

N1030 G0 G90 G54 X.25 Y-.25 S2139 M3

N1040 G43 H91 Z.1

N1050 G99 G81 Z-.1 R.1 F4.11

N1060 X.75

N1070 X.25 Y-.75

N1080 X.75

N1090 X.5 Y-.5

N1100 G80

N1110 G55 X.25 Y-.25 Z.1

N1120 G99 G81 Z-.1 R.1 F4.11

N1130 X.75

N1140 X.25 Y-.75

N1150 X.75

N1160 X.5 Y-.5

N1170 G80

N1180 G56 X.25 Y-.25 Z.1

N1190 G99 G81 Z-.1 R.1 F4.11

N1200 X.75

N1210 X.25 Y-.75

N1220 X.75

N1230 X.5 Y-.5

N1240 G80

N1250 M5

N1260 G91 G28 Z0.

N1270 G28 X0. Y0.

N1280 G90

N1290 M30

%

---

HTH

[Philcott]

Jorges,

 

I am not a mill guy but I believe you go to Mill toolpath, transform,check toolplane, highlight assign new, start 0, increment 1, highlight copy source operations and unselect disable posting in source operations, set values on translate tab. Click ok

 

Check for errors. Remember I'm not a mill guy.

 

I am sure someone more adept will fill in the blanks but this should get you started on the path .

 

Phil

[connormac]

mpsubrep.pst will do it for you. You can also set it up to do a block delete on the last 2 subs. This way you can prove out the program on 1 vise then run all the vises.

[jorges]

I will try that today

Thanks guys

[RDub]

Hey Connor,

 

where can I get mpsubrep.pst? It mentions it in my mpMaster control def, but it didnt come with it.

[Guest]

Right here

 

http://www.emastercam.com/posts/mpsubrep/mpsubrep.html