EIA/ISO Sample Code for Mazatrol Matrix

[Justin Beebe at Folsom Tool]

Can someone please post some sample code of EIA/ISO for Mazatrol Matrix Integrex IV. We are trying to program this machine using mastercam for the first time and need some sample code.

 

Thanks

[mayday]

what kind ? turn, mill, 5 axis ?

[mayday]

turn on main spindle

 

(T2 | OD ROUGH RIGHT - 80 DEG. )

G123.1

M901

M202

G53.5

T2 T006 M6 D001

G28 U0. V0.

G28 W0.

M250

G0 B90.

M251

G53.5

G18

G50 S6000 R1

G96 S180 M03 R1

G0 X9.555 Z2.132

G99 G1 X8.1375 F.005

G0 Z2.162

X9.555

Z2.108

G1 X8.1375

G0 Z2.138

X9.555

Z2.084

G1 X8.1375

G0 Z2.114

G28 U0. Y0.

G28 W0.

M01

[mayday]

turning on sub spindle

 

 

N9

(| OD ROUGH LEFT - 80 DEG. DNGP-431)

( ROUGH FACE & TURN)

G123.1

M902

M302

G53.5

T9.01T005M6D009

G28U0.V0.

G28W0.

M250

G0B180.

M251

G53.5

G18

G50S6000R2

G96S175M304R2

G0 X7.7457 Z-.3404

X7.675 Z-.305M8M153

G99 G1 X3.9578 F.004

X3.9278 Z-.32

X3.5238

G0 X3.5945 Z-.3554

X7.7457

Z-.3254

X7.675 Z-.29

G1 X3.9878

X3.9378 Z-.315

G0 X4.0085 Z-.3504

X7.7457

Z-.3104

X7.675 Z-.275

G1 X4.0121

Z-.2779

X3.9678 Z-.3

G0 X4.0385 Z-.3354

X7.7457

Z-.2954

X7.675 Z-.26

G1 X4.0121

Z-.2779

X3.9978 Z-.285

G0 X4.0685 Z-.3204

Z-.5

M9M154

G28U0.Y0.

G28W0.

M05

M00

M00(CHECK INSERT)

[Justin Beebe at Folsom Tool]

Thanks Wes this is for a Mill Turn Machine. We would still like to see more code if anyone has any.

[mayday]

drlling on main

 

make note !!1 always use G68 rotate and only use milling toolpaths, not c axis paths

 

N3

(T3 | 3/64 FLAT ENDMILL | LEN. - 3. | DIA. - 3. )

G122.1

M902

M300

G110 C2

G53.5

T3 T004 M6 D003

G28 U0. V0.

G28 W0.

G97 S8300 M203

M248

M250 M312

G98 G0 B102. C280.

M251 M311

G53.5

G111

G68.5 X0. Y0. Z0. I0. J1. K0. R102.

G0 G17 X.55 Z3.

Y0.

G83 Z-1.9327 R4.8729 Q.02 F5. M311

G80

G69.5

G28 U0. Y0.

G28 W0. M205

M01

[Justin Beebe at Folsom Tool]

Wes for the tool change why don't you use Tool ID Code for example:

 

T006.01 for tool type A

[mayday]

operators set up tool data here

I have every type of path you can think of, we have the same machine. let me know what you need to see

[Jeremy Herron@DBS Solutions™]

+1 to everything Wes said, and the only reason you would need a tool i.d. code for a milling tool is if you had more than 1 definition of the same tool with a different length offset.

[mayday]

here is a snip of 5 axis

 

 

G28 U0. Y0.

G28 W0.

 

N1

(3/16 BALL ENDMILL )

G122.1

M901

M200M300

T24 M6 D024

G30 P4 U0. V0.

G30 P4 W0.

M511(SYNCRO)

G97 S2852 M203

M248

G52.5 (MAZATROL COORDINATE SYSTEM CANCEL)

G10 L12 P[#51999] R[#[61000+#3020]/2] (TOOL RADIUS)

G10 L10 P[#51999] R#[60000+#3020] (TOOL LENGTH)

(WORK OFFSET G54 DATA SETTING)

G10 L2 P1 X#50700 (WORK OFFSET G54 X__)

G10 L2 P1 Y0.0 (WORK OFFSET G54 Y0.0)

#3200=3 (Z AXIS PARAMETER ROW OF S23)

#500=[#3223/100000] (#500 CAPTURES Z IN S23 PARAMETER)

G10 L2 P1 Z[#9101+[#500]] (WORK OFFSET G54 Z__)

G10 L2 P1 C#9102 (WORK OFFSET G54 C__)

G10 L2 P1 B0.0 (WORK OFFSET G54 B0.0)

G54

M250 M212

G98 G0 B100.5515 C11.3506

M211

G0 X6.0 Z-.4 G43.4 H24

X.3872 Z-.3869

Y-.6117 M8

G98 G1 X-.0241 Y-.5291 F100.

X-.0342 Y-.5008 Z-.3857 F6.

X-.039 Y-.4868 Z-.3841 C11.3483 B100.4925

X-.0451 Y-.4716 Z-.3821 C11.3461 B100.4412

X-.049 Y-.4617 Z-.3808 C11.3446 B100.4057

X-.0527 Y-.452 Z-.3796 C11.343 B100.369

X-.0562 Y-.4424 Z-.3784 C11.3414 B100.3314

X-.0596 Y-.433 Z-.3773 C11.3397 B100.293

X-.0628 Y-.4236 Z-.3762 C11.3379 B100.2538

X-.0662 Y-.4134 Z-.375 C11.3357 B100.2084

X-.0693 Y-.4034 Z-.3738 C11.3335 B100.1621

X-.0724 Y-.3935 Z-.3727 C11.3312 B100.1153

X-.0753 Y-.3839 Z-.3717 C11.3288 B100.0673

X-.0806 Y-.3649 Z-.3696 C11.3238 B99.9698

X-.0854 Y-.3466 Z-.3677 C11.3184 B99.8698

X-.088 Y-.3359 Z-.3666 C11.3149 B99.8087

X-.0905 Y-.3254 Z-.3656 C11.3114 B99.747

X-.0928 Y-.3151 Z-.3646 C11.3077 B99.6844

X-.0949 Y-.3049 Z-.3636 C11.3039 B99.6214

X-.0974 Y-.2928 Z-.3624 C11.2992 B99.5448

X-.0995 Y-.281 Z-.3613 C11.2942 B99.4671

X-.1016 Y-.2695 Z-.3603 C11.2891 B99.389

X-.1034 Y-.2581 Z-.3593 C11.2838 B99.3103

X-.1051 Y-.247 Z-.3583 C11.2783 B99.2309

X-.1066 Y-.236 Z-.3573 C11.2726 B99.151

X-.108 Y-.2252 Z-.3564 C11.2668 B99.0709

X-.1092 Y-.2146 Z-.3555 C11.2608 B98.9903

X-.1103 Y-.2047 Z-.3547 C11.2549 B98.9136

X-.1113 Y-.1949 Z-.3539 C11.2489 B98.8365

X-.1129 Y-.1758 Z-.3524 C11.2363 B98.6814

X-.114 Y-.1568 Z-.3509 C11.2227 B98.5215

[crazy^millman]

How are you running the tools? Eia or Mazatrol for the control of them? Are you planning on using the G68 for your coordiate shift? The main things are the codes from main to sub spindle then the milling. Getting all that sorted out is the biggest thing beside maybe in you are planning on doing canned cycles for the turning operations.

[crazy^millman]

Jermeny, I had many tool defintions for the same milling tool. I would have a main spindle and a sub spindle one. I would also have different ones for chasing hole sizes with endmills.

[mayday]

Justin, did you get your pst from In-House? if so you should be good to go

[Jeremy Herron@DBS Solutions™]

Jermeny, I had many tool defintions for the same milling tool. I would have a main spindle and a sub spindle one. I would also have different ones for chasing hole sizes with endmills.

 

I did not mean to imply that you would not need one sometimes. I was just saying that was when you would need to call one.

 

+1 one to the inhouse post.

 

Another thing to be aware of, unless this has changed on the newer models, if you are going to do 5-axis work on the sub spindle , you have to sync the spindles and tell the machine you are working on the main spindle.

 

Ron and Wes, Do you Guys use a G50 workshift for moving your Z between spindles or G53.5 Z[#variable]?

[mayday]

On the old mark4 we use the G50

We have 4 new I series machines and they are mill based. So I can set any work offset I want. Normally G54 on main and G55 for sub. They are way cool to program compared to the old style slant bed Integrexes. I use multi axis paths for all milling on the new ones, just because they play better with G43.4

[crazy^millman]

I used the G54 and G55 and well as many others.

[Justin Beebe at Folsom Tool]

Thanks for the replies everyone. I am asking these questions to help a co-worker. When I talk to him monday I will be able to give you guys more information. It would also be helpful to us if someone would be willing to answer some questions over the phone.

 

Thanks again

[crazy^millman]

Justin, email me and I will be glad to assist.