Mazak integrex 300 stock transfer

[Joels]

Hello. We purchased a new Mazak Integrex 300S. I am trying to do a part cutoff and a part transfer to the second spindle. First i need to call up the cutoff tool and have it move out of the way of the second spindle. Does anybody know how to do this? I am using x with a post from in house solutions.

[crazy^millman]

The post from them has this pretty much dialed in. What happened when you used the code for the transfer cycle out on the machine?? Is anyone from CCC helping you get this dialed in or our you on your own??

[Joels]

Millman. CCC has helped alot but i also have to figure it out on my own so i figured i would come here. I have been here for a long time but usually just read. Mazak wants me to use MAZATROL but i can do it all in mastercam alot faster. The spindle transfer from the post works perfect but i need to stage the tool out of the way before i bring in the second spindle. This is what i am working on now. I was reading the post doc and it says how to stage the tool, now i am just trying it out but someone out there might have some quick tips for me?

[crazy^millman]

Ok so have you looked at the point toolpath with the tool in question to set it at the position you are looking for? I program our Integrex E410-HS with Mastercam and we make some pretty complex parts.

[Joels]

I looked at the point tool path and tried it but if you look in the transfer operation it has a box to make a tool callup and move to get it out of the way so that is what i am trying now. i read the post doc and it said it would do this now i have to look up what g30 means (docs are at work) if it means go to programmed z zero i am in luck if not i will keep trying. I assume you use point programming to assure the tool is clear?

[Joels]

Millman i do appreciate your replies!!!!

[DavidB]

I do my moving of the lower turret by Manual entry toolpath.

Make sure it has (lower) code then *

 

Example:

(lower)

W-455.

M950

*

 

You can put as much detail in there as you want

 

(lower)

G28 U0. W0.

T009009

W-455.

*

 

 

HTH

[crazy^millman]

Yes just to know you are where you want to be. Our machine works different than yours so I do not have to go through the struggle you do. I will try to put something together tomorrow and show you what I think should work on your machine. Glad to help anytime I can. Have A good night.

[Joels]

Davidb. I tried the idea you had but i cant get the code to be placed in the program where it needs to be. I am at work now so i am going to look up G30 and that might work.

 

Thank you

[Joels]

i also am having problems getting the tool to machine the right side spindle too!

[Joels]

Anybody have a idea why i cant seem to machine on the right spindle?

[crazy^millman]

What kind of problems are you having? Did you pick the right turret set-up? Did you pick the tools facing the correct position? Did you set the tools up for the right turret? Are you doing the stock transfer for your geometry or are using one set of geometry for your main and sub spindle work? Are you using the Mazatrol letters in your programming and do you have them set-up right in the machine? Are you using one workoffset for each spindle or trying to use one workoffset for both spindle? How much training have you got on Mill/Turns and programming in Mastercam?

[DavidB]

As Crazy said make sure the correct axis combo is selected.

[Joels]

I have very little expirence working with mastercam and a mill turn. I have been trying to figure out the part cutoff and transfer but i havent done that yet. I am working with Rob at Cad-cam to reslove the issues. Currently i am creating a Mazatrol program which has a spindle transfer in it that was created by a Mazak app engineer. I creat the complete program for the first spindle in mastercam then call it up in the Mazatrol program as a sub program and this is working perfect. So the first spindle is complete and then we do a spindle cutoff, transfer and stuff ( we are doing bar work) so then i create a separate mastercam program for the sub spindle and call it up after the transfer with the Mazatrol program specifying the second head will be used. I execut the mazatrol program and it calls the sub program and the tool loads and loads the right direction and the subspindle turns on and the b axis head moves toward the main spindle. I have looked at the cnc program from mastercam and checked all the codes and they look good. so i have no idea why this is happening. I want to do all the programming in mastercam but i have a new machine on the floor and i cant run it because i cant program it so it is frustraiting. i can post the program or the code it you want to see it. I do pick the axis combos, tool direction so i am confused.

[Joels]

here is the cnc code i get from mastercam when i program the second spindle.

(PROGRAM NAME - H36160532401 OP-2 DATE=DD-MM-YY - 05-06-08 TIME=HH:MM - 04:56 )

(MASTERCAM - X)

(MCX FILE - C:MCAMXMCXLATHEMAZAK H36160532401 OP-2 .MCX )

(POST DEV - IN-HOUSE SOLUTIONS)

(T1 | OD ROUGH RIGHT - 80 DEG. | ID CODE - .02)

 

G28 U0. Y0.

G28 W0.

(G50 Shift Parameters Used)

 

N1

(T1 | OD ROUGH RIGHT - 80 DEG. | ID CODE - .02)

(ROUGH AND FINISH FACE)

(TOOLPATH GROUP - TOOLPATH GROUP-1)

G123.1

M902

M302

G53.5

T1.02 M6

G28 U0. V0.

G28 W0.

M250

G0 B90.

M251

G53.5

G18

M8

M153

G97 S1000 M304 R2

M248

G0 X3.185 Z-3.92

G99 G1 X-.0625 F.007

G0 Z-4.02

X3.185

Z-3.82

G1 X-.0625

G0 Z-3.92

G28 U0. Y0.

G28 W0.

(ROUGH AND FINISH BACKSIDE)

T1 D001

X2.9537 Y0. Z-3.92

Z-4.02

G1 Z-3.92 F.01

Z-2.9365

X3.1264 Z-2.8501

X3.2678 Z-2.9208

G0 Z-4.02

X2.781

G1 Z-3.92

Z-2.955

X2.8825

G2 X2.9408 Z-2.9429 I0. K.0413

G1 X2.9737 Z-2.9265

X3.1151 Z-2.9972

G0 Z-4.02

X2.6083

G1 Z-3.92

Z-2.955

X2.801

X2.9424 Z-3.0257

G0 Z-4.02

X2.4356

G1 Z-3.92

Z-3.067

G2 X2.47 Z-3.0288 I-.034 K.0383

G1 Z-2.955

X2.6283

X2.7697 Z-3.0257

G0 Z-4.02

X2.2629

G1 Z-3.92

Z-3.08

X2.3675

G2 X2.4556 Z-3.0549 I0. K.0513

G1 X2.597 Z-3.1256

G0 Z-4.02

X2.0902

G1 Z-3.92

Z-3.08

X2.2829

X2.4243 Z-3.1507

G0 Z-4.03

X1.9175

G1 Z-3.93

Z-3.83

G2 X2.02 Z-3.7788 I0. K.0513

G1 Z-3.6637

Z-3.08

X2.1102

X2.2516 Z-3.1507

G0 X7.049

M9

M154

G111

G28 U0. Y0.

G28 W0.

M305

M30

[crazy^millman]

Joels I am in Brea, would it be ok with whoever you work for for you to come to our shop and I sit down with you an show you some different things about programming in Mastercam with regards to Mill/Turns? Once we get you more understanding with things then I would be glad to come over to your shop and help you dial in a eia transfer program. We use this on our machine right out of Mastercam. All the operator has to do is put in the W value and we are done. Here is what we use on our Integrex it is different, but maybe it will help.

 

code:

---

N100 (CHUCK TRANSFER UNIT)

M307

M202M302G10.9X1

G20G80G40G17G90G94G98

G91G53G0X0.

G91G28X0.

G91G53G0X0.

G91G28X0.

G91G28Y0.

G91G28Z0.

G91G28W0.

M108

G0B0

M107

M0(BLOW OUT JAWS/PART)

#100 =

G17G40G80G90G94G98

G94M540M306

M200M300

G0C0.U0.

M210M310

M508

G90

G0W[#100 +.5]

G1W#100 F10.

G55

G4X2.

M307

G4X5.

M206

G4X5.

G91G30W0

M541

M212M312

M01

---

HTH