O/T Another Mazak Integrex Question

[dan m]

Hi All,

 

Let me start by saying I don't need a post. What I have is a 1987 Mazak Integrex 40-atc m/c turning center. We are looking to do more g-code programming on the machine and have a post but the machine don't like the all the code my post puts out. There are some g-code errors and things of that nature. What I was wondering is if someone could send me a short program that there integrex uses preferably with a turning and milling op. so I can try it and try to figure out where to start editing my post. Any help would be appreciated.

[RStuart]

Did you check and see if the machines parameters were changed so that it would use the correct set of G-codes for your post. We have 2 newer Integrex's, not sure how they differ from yours. The only problems I have had with my post were 6 digit tool numbers that I didn't need and it would not machine arcs correctly unless they were broken up into sections, these were both simple fixes in the post. If you still need a program I am sure I can hook you up with one. Let me know.

 

[ 10-31-2003, 07:09 AM: Message edited by: RStuart ]

[Simtech]

Dan m,

 

From out experience working with Dave from In-House to develop the Integrex post ... buy it! After close to a year in development plus macros used for plane mapping and so on, you would be much better off to get it from your dealer IMHO.

 

Luc

[dan m]

Thanks for the replys,

For some reason are machine don't understand the following lines that my post puts out

G28 Y0

G28 U0 W0

 

I wonder if there needs to be a G91 in there?

It also don't like the Y moves at all so I delete them out.

 

My tool changer looks like T0404.00 when it should look like T0404.9

 

These are just some of the things, thats why I asked if some one had code I could try because I'm shooting in the dark at what this machine likes and dislikes.

[Harryman]

Good morning Dan,

 

Does your machine have a Y axis?

 

G28 U0 V0 W0 works on our machine in any combination.

 

Looking at your code again I see G28 Y0, try V0.

 

I didn't answer earlier because yours is the older style and I don't know what you need.

 

Hope this helps.

 

Lathe code:

(TOOL - 4 OFFSET - 4)

(LFINISH GNL OUT 80 B .032 INSERT - CNMG-431)

( PRE FINISH FACING )

N200 G28 U0.

G28 W0.

M202

T0404.1302 B5***this B is tool stage not B axis

G53

G18

G97 S43 M3

G99

M248

G0 X26.7 Z-.06 M153

G50 S800

G96 S300

G99 G1 X26.5 F.012

Z-.0593

G2 X26.3775 Z.002 R.0613

G1 X23.9975

X22.6895

X22.4401

Z.052

M154

G28 U0.

G28 W0. M5

M01

 

Mill code using G12.1:

(TOOL - 38 OFFSET - 38)

(FACE CONTOUR 5/8 HELICAL INSERT ENDMILL)

( ROUGH MILL 10 INCH HOLE )

N900 G28 U0.

G28 W0.

M200

T3838.0008 B38 ***tool stage

G53

M250

G0 B0. **** B axis

M251

G17

M212

G97 G0 C0.

G98

M211

G12.1

M153

S990 M203

M248

G0 X4.6825 Y0. Z.25

Motions deleted

Z.1 C0.

G1 Z-.1249 F2.8

G3 X0. Y4.6825 R4.6825 F3.7

G0 Z.25

G13.1

M154

Y0.

G28 U0.

G28 W0. M205

M00

 

Milling diametrical X values:

(FACE CONTOUR 3/4 FOUR FLUTE ENDMILL)

( FINISH 2.76 HOLES )

G20

N100 G28 U0.

G28 W0.

M200

T3737.0002 B37

G53

M250

G0 B0.

M251

G17

M212

G97 G0 C0.

G98

M210

M8

S305 M203

M248

G0 X20.49 Z.65

Y0.

Z.05

G1 Z-.98 F10.

G41 X20.61 F1.8

G3 X18.6 Y1.005 R1.005

X16.59 Y0. R1.005

X18.6 Y-1.005 R1.005

X20.61 Y0. R1.005

X20.6099 Y.01 R1.005

G1 G40 X20.4899 Y.0094 F10.

G0 Z.65

M9

Y0.

G28 U0.

G28 W0. M205

M30

[dan m]

Thanks Harry,

I appreciate your reply. I will probably try it tomarrow night. We have a Y axsis but we don't use it. Your code should give me a place to start.

[Mick]

If you're not using your Y axis, could I have it please? I could sure do with it on our Okuma LB25!

I'd send you a coouple of dozen beer!

Sorry, I couldn't resist a crack, as its the end of the day, and I'm tired from staring at a computer screen all day

Hehehehe...

[dan m]

Mick,

You can have it. We had the tech from Mazak come out to show us how to use it and after 1 look at it he told us it wasn't worth the trouble. According to him it's to old and not reliable like the new one's.

 

Harry,

Thanks for the code there was alot of m codes our machine dont like but it got me pointed in the right direction (i think so far).

I appreciate all the help from everyone out here on all my questions. It's used to be hard to get things done on third shift till I found this forum.