Need to see G-Code Output

[TobyAxis]

Ok this is my first question on this forum. Can someone post a G-Code program for a Mazak MSY 200 with a Fusion 640T Control.

 

I'm having trouble with the tool calls for regular turning tools as well as the Live Tooling when doing C Axis machining. These guys are using Mazatrol Programs because they don't understand G-Code. I understand G-Code but not Mazatrol. Ha Ha Ha what a nice combo.

 

Is it a T0101.1.1 call for Turning Tools or a regular T0101 like a Fanuc/Yasnac?

 

Any help is greatly appreciated as this Lathe is kicking my butt.

 

BTW: Don't forget to add some good jokes too. A laugh would be good about now.

[Guest CNC Apps Guy 1]

crazy_millman is one of our resident Integrex Experts.

[Psychomill]

Toby... you've got mail....

 

Tool calls break down like this for 640T (which is a Quick Turn machine right? If its a 200MSY)

 

T0101.1 First 2 digits is tool number, next two digits are offset number. The value after the decimal would be the Tool ID code from the tool data. If you're using 6 digit tool system, it would be: Txxxyyy.1

 

"T0101.1.1" would be something you might see on an Integrex. The middle digit would be tool direction.

 

With all of the Mazaks you have, you should get a hold of the books. Theres alot of info in there on EIA programming. Although for these machines, learning the Mazatrol would really be ideal. Not as difficult as it looks and you'll be surprised by it.

[Hardmill]

quote:

---

BTW: Don't forget to add some good jokes too. A laugh would be good about now.

---

Here you go

 

 

 

PEACE

[TobyAxis]

Thanks for the insite guys. So what your saying is that I can use the Tool Data 2 Page for the milling and Drilling (Face and Cross X Axis).

 

Ex.

 

O00000552(INGRAVING)

G20

M201

C6.5

G0T202(this could be T202.2)

G54G00X8.Z8.

M62

G96

S4500M203

G54X2.1Z-.1Y-.045

G99M08

G1X2.044F.003

Y.045

Z-.1226

Z-.1265Y.0446

Z-.1302Y.0437

Z-.1337Y.042

Z-.1369Y.0398

Z-.1397Y.0368

Z-.142Y.0338

Z-.1436Y.0303

Z-.1446Y.0264

Z-.145Y.0225

Z-.1446Y.0186

Z-.1436Y.0147

Z-.142Y.0113

Z-.1397Y.0082

Z-.1369Y.0052

Z-.1337Y.003

Z-.1302Y.0013

Z-.1265Y.0004

Z-.1224Y0.

Z-.1

G0X2.1

 

This is an OD Engraving Program from the control memory. Does anyone have a Face Milling Program to share that won't violate a Confidentiality Agreement? Just a Simple Pocket on the Face of a cylindrical part will do nicely.

 

Thanks Again

 

BTW: Sorry for cluttering this Forum with Mazatrol Questions.

[Psychomill]

Calling Crazy_Millman.... !!!

 

As James said, he's the resident expert... they're a couple others that knows this stuff pretty well too...

 

In the future though, might at least label these types of questions as "Off Topic" or "OT". Or post them in the Off Topic forum. Unless of course, you have specific questions on maybe modifying a post to work for the machine....

 

[crazy^millman]

Sorry Guys just seeing this thread. Ok this is a Quick turn machine with C axis and Y axis milling. I have the books for this machine in PDF so send me and email and I will help you there.

 

I am assuming you have the Sub spindle as well. With Mazatrol and Eia the machine needs to have certain paramters set-up to use the toolpages from either a certain way. F93 and F94 are some of the paramters that control this. The machine has 2 offset page one that Mazatrol uses and one that Eia uses. I like ot set the parameters up so that you only use the Mazatrol one that way the tool eye update your tooloffset and you only need to worry about adjusting one set of tool offsets. The integrex works differently than the Quick Turn, but here is an Example I got at hone from Mazak.

 

code:

---

N100 G20

(PROGRAM NAME - 2546 DATE=DD-MM-YY - 14-09-04 TIME=HH:MM - 08:08 )

(TOOL - 1 OFFSET - 1)

(MATERIAL STOP INSERT - CNMG-432)

N102 M302

N104 G28 U0. W0.

N106 G0 T0100

N108 G0 T0101

N110 M05

N112 G0 X1. Z.01 M9

N114 M00

N122 Z.1

N124 T0100

N126 G28 U0. W0.

N128 M01

(TOOL - 5 OFFSET - 5)

(OD ROUGH RIGHT - TNMG-332 INSERT - TNMG-332)

N130 M302

N132 G28 U0. W0.

N134 G0 T0500

N136 G0 T0505

N138 G97 S191 M03

N140 G0 X10. Z.1 M8

N142 G50 S3000

N144 G96 S499

N146 Z.005

N148 X1.5

N150 G99 G1 X-.0625 F.01

N152 G0 Z.105

N154 G96 S450

N156 X1.1616

N158 Z.06

N160 G1 Z-.8975 F.012

N162 X1.3 Z-.9667

N164 X1.4414 Z-.896

N166 G0 Z.06

N168 X1.0231

N170 G1 Z-.0696

N172 G3 X1.0386 Z-.0924 R.0413

N174 G1 X1.07 Z-.5932

N176 G3 Z-.5945 R.0412

N178 G1 Z-.8652

N180 G3 X1.1208 Z-.8771 R.0413

N182 G1 X1.1816 Z-.9075

N184 X1.323 Z-.8367

N186 G0 Z.06

N188 X.8847

N190 G1 Z-.0016

N192 X1.0136 Z-.0641

N194 G3 X1.0386 Z-.0924 R.0412

N196 G1 X1.0431 Z-.1641

N198 X1.1846 Z-.0934

N200 G0 X10.

N202 Z.1

N204 M9

N206 T0500

N208 G28 U0. W0. M05

N210 M01

---

The couple of thing I have done on the quick turn shows me that .1 uses the 2nd tool for the back work at the same turret location and without it for the tool call it is the front of the turret. Like below:

code:

---

N428 Z.1

N430 M9

N432 T0800

N434 G28 U0. W0. M05

N436 M01

N438 (RE-POSITION - RIGHT SPINDLE)

N440 M202 M302(MILL MODE OFF & MAIN SPINDLE SELECT)

N442 M19(MAIN SP ORIENT)

N444 M319(SSPINDLE ORIENT)

N446 M306(SSPINDLE UNCLAMP)

N448 G0 B-20.2725

N450 M307(SSPINDLE CLAMP)

N452 M511(MAIN & SSPINDLE SYNCH START)

(TOOL - 9 OFFSET - 9)

(PARTING .188 WIDE INSERT - NONE)

N454 M302

N456 G28 U0. W0.

N458 G0 T0900

N460 G0 T0909

N462 G97 S103 M03

N464 G0 X10. Z.1 M8

N466 G50 S3000

N468 G96 S270

N470 Z-2.398

N472 X1.5

N474 G1 X-.008 F.0018

N476 G0 X1.5

N478 X10.

N480 Z.1

N482 M9

N484 T0900

N486 G28 U0. W0. M05

N488 M01

N490 M06

N492 G0 B0.

N494 M07

(TOOL - 1 OFFSET - 1)

(T0101A CNMG 432 SUB SPINDLE INSERT - CNMG-432)

N496 M300 M512

N498 G28 U0. W0.

N500 G0 T0100

N502 G0 T0101.1 <----sub spindle ###########################

N504 G50 W-18.0725

N506 G112 G97 S191 M304

N508 G0 X10. Z-.1 M8

N510 G112 G50 S3000

N512 G112 G96 S499

N514 Z0.

N516 X1.5

N518 G1 X.625 F.01

N520 G0 Z-.1

N522 G96 S450

N524 X1.2407

N526 Z-.06

N528 G1 Z.937

N530 X1.3 Z.9667

---

I also included some tranfer code I got as well. We have a multi-year Contract for this machine and are only running one part, but I will help you anyway I can. Mazatrol is very easy to learn and use the biggest thing is understand it is backwards to what you think. Z on the main spindle is Z positive towards the chuck in Mazatrol and Z towards the chuck in Eia is Z negative. It is the oppsite of that on the sb spindle. The Z towards the chuck is Negative on the sub spindle and in Eia Z is postive towards the chuck on the sbu spindle. Also you can use the Mazatrol program for location and your set-up page and then call an eia program from there to take advangate of this since the machine does not use workoffsets to establish a position in which to run the program. You can use the Set-up page for an eia program, but then you can not use the Backplot in Mazatrol to test your eia programs.

 

Post up spefic questions I know there is a spefic post made for this machine out there. You might be able to take the Mplfan and modify to use for your use.

 

HTH sorry for the length.

[crazy^millman]

I think this falls under A spefic Mastercam Forum Question unless you are not using Mastercma in which to post code from for the Machine.

[TobyAxis]

WOW, that clears a lot of things up for me. Thanks a lot Ron. I'll be sending you my email address ASAP. I will enjoy the Mazak PDF files. I'll put them on my Lap Top and take them to work to use while working on this.

 

BTW Next time I'll post a question in the Off Topic Forum LOL.

 

I still have lots to learn about Mazak and MC.

 

Thanks for everyones help!!!!!!