Programming a Mazak using Mastercam

[G Caputo]

I have searched and searched and read and read on this forum and I am in need of some help getting our vertical mill to run. It is a V550 with a M32 control made around 1990. I have a few questions I hope you guys can help me with.

 

1) As stupid as this sounds, what is the

definition of EIA vs ISO programming? It's all

grouped into one button om the machine and

looks as though the control wants to see an

ISO extension on the file to run. Is this

correct?

 

2) I have serched and read through the previous

posts talking about using the Mazatrol's tool

table when posting ISO/EIA programs to it and

for the life of me can not get it to work.

Jack Mitchell had to previous posts about

changing the f91-f95 parameters and I am

having no luck getting the machine to

recognize this. Can I use only the Mazatrol

tool table to program the machine successfully

with Cutter comp set at the control this way?

Do I need to use some kind of different tool

list in the machine?

 

3) I post a program to the control using either

one or two tools and the machine runs and

moves but the toolchanger brings out no tool

so I have (tool 0 maybe?) an empty spindle

spinning.

 

Here is just a bogus rectangle I programmed trying to get the machine to run.

 

105

(DATE - 22-02-06 TIME - 10:25)

N25

G20

G0G40G80G90G94G98

G0G28G91Z0.

G0G28X0.Y0.

(1-1/2" APFT TOOL - 25 DIA. OFF. - 25 LEN. - 25 DIA. - 1.)

(ROUGH ID)

T25M6

G0G54G90X3.6667Y0.S100M3

G43H25Z5.

Z.1

G1Z-1.F10.

G41D25Y-1.3333F30.

G3X5.Y0.J1.3333

G1Y5.

X-5.

Y-5.

X5.

Y0.

G3X3.6667Y1.3333I-1.3333

G1G40Y0.

G0Z5.

M5

G0G28G91Z0.

M01

N14

G0G40G80G90G94G98

G0G28G91Z0.

(1" APFT TOOL - 14 DIA. OFF. - 14 LEN. - 14 DIA. - 1.)

(ROUGH ID)

T14M6

G0G54G90X3.6667Y0.Z5.S100M3

G43H14Z5.

Z.1

G1Z-1.F30.

G41D14Y-1.3333

G3X5.Y0.J1.3333

G1Y5.

X-5.

Y-5.

X5.

Y0.

G3X3.6667Y1.3333I-1.3333

G1G40Y0.

G0Z5.

M5

G0G28G91Z0.

G0G28X0.Y0.

M02

%

 

I know very little about Gcode as all of the machines I program for are Heidenhain conversational, so maybe I am missing something very simple here. I got from previous posts that I needed to get rid of the M30 at the end and throw in an M02. No percent sign is allowed at the top, but it needs one at the bottom. The program above is beeing drip fed (Thanks to this forum )from a PC as that is how we will be running programs through the machine if that makes a difference. Any help would be GREATLY appreciated to help me get this thing up and running using mastercam.

[snowman]

I just changed one of my mazaks

parameters with a m32 control to

run the mazatrol library. I changed

f92 and f93 to this.

f92 10101000

f93 00001000

 

You may want to try to stage a tool

to see if this helps your tool changing

problem

 

code:

---

105

(DATE - 22-02-06 TIME - 10:25)

N25

G20

G0G40G80G90G94G98

G0G28G91Z0.

G0G28X0.Y0.

(1-1/2" APFT TOOL - 25 DIA. OFF. - 25 LEN. - 25 DIA. - 1.)

(ROUGH ID)

T25M6T30

G0G54G90X3.6667Y0.S100M3

---

If you want a can send you a program

to look at.

[G Caputo]

Snowman,

If you don't mind, I would really appreciate if you could send me something that runs for sure so I can compare and make this thing work.

[snowman]

Greg,

check your mail.

[mayday]

quote:

---

check your mail.

---

scary

 

 

[snowman]

quote:

---

scary

---

Dont forget who taught me.

 

[Guest SAIPEM]

EIA and ISO are the standards organizations.

 

Tool Change needs to be T25T14M06 if you want to stage the next tool.

 

If you don't then the M06 has to be on a line following the tool call.

T25

M06

 

 

If you are using Mazatrol Tool Data and WEAR or REVERSE WEAR as the cutter comp type in Mastercam, then you need to lie in the Mazatrol Tool Data for the ACTUAL diameter of the tool and enter the smallest allowable value.

 

 

If you want the machine to run completely like a Fanuc control then you need to use the EIA offset data page for Tool Length and Diameter Comp.

 

You need to consult the Mazatrol Parameter manual for EIA related parameters.

 

Review F80,F84,F88,F89 in addition to the previous parameters listed.

[Jack Mitchell]

quote:

---

looks as though the control wants to see an ISO extension on the file to run. Is this

correct?

---

The correct extension for a Mazatrol control prior to the 640 Fusion is .NC

Since the introduction for the 640 control the extension is .EIA

(these are both just ascii text).

 

Regards, Jack

[G Caputo]

quote:

---

Tool Change needs to be T25T14M06 if you want to stage the next tool.

 

If you don't then the M06 has to be on a line following the tool call.

T25

M06

---

That works exactly as descibed and I actually have a tool rotating in the spindle now.

 

quote:

---

The correct extension for a Mazatrol control prior to the 640 Fusion is .NC

---

I put a .iso extension on the end and it took it. I helped one of my buddies get a haas running recently and it wouldn't take any kind of extension at all This mazak seems to not care about the .iso extension, but I will throw a .nc and see what happens.

 

A big thanks to all of you, and thanks for the emails snowman. I've got to try out some tools for the rest of the day but I will get back at the Mazak in the morning and see what I can make happen. Thank you all for getting me off on the right track!

[G Caputo]

I have a few more issues if any of you fine folks care to spread your knowledge my way. I have made a very simple program that uses two tools. I am not prestaging them and have been able to get my post to do want I want it to do, I am just not sure what it is that I do want it to do. If I post out these to operations seperately, each program runs fine, but when I post it as one program, when it goes to do a toolchange, I get an error "296 toolchange imp. (no axis in atc)". What is either missing from or needs to be added to the code for this to work? I also have the machine understanding the mazatrol tool table when running eia/iso programs as described in snowman's post. My question is, does the machine care if it sees the "h" and "d" codes in the program with the Mazatrol tool table being utilized?

 

O1(PROGRAM - 1)

(DATE - 24-02-06 TIME - 09:54)

G20

G0G40G80G90G94G98

G0G28G91Z0.

G0G28X0.Y0.

(5" CARBOLOY OCTOMILL TOOL - 15 DIA. OFF. - 15 LEN. - 15 DIA. - 4.92)

(SKIN BOTTOM TO +.005")

T15

M6

G0G54G90X-14.Y2.3975S398M3

G43H15Z5.

Z.105

G1Z.005F32.6

X14.

G0Z1.

Y-2.3975

Z.105

G1Z.005

X-14.

G0Z5.

M5

G0G28G91Z0.

M01

G0G40G80G90G94G98

G0G28G91Z0.

(2-1/2" X 1-5/8" DOC DAPRA SQUARE SHOULDER TOOL - 8 DIA. OFF. - 8 LEN. - 8 DIA. - 2.5)

(MILL BOTTOM TO FINISH)

T8

M6

G0G54G90X-14.Y2.4375Z5.S917M3

G43H8Z5.

Z.1

G1Z0.F37.

G41D8Y-.0625

X14.

G40Y2.4375

G0Z1.

Y-2.4375

Z.1

G1Z0.

G41D8Y.0625

X-14.

G40Y-2.4375

G0Z5.

M5

G0G28G91Z0.

G0G28X0.Y0.

M02

%

 

Any help is greatly appreciated.

[Guest SAIPEM]

You aren't specifying the XY position for the second toolchange.

 

G0G91G30Z0.

G0G91G30X0.Y0.

 

You should be using G30 instead of G28 for the returns.

G30 is the G-Code for the Return to Tool Change Reference Point on a Mazak.

[tryon]

With the Mazatrol tooldata, G43,H and D codes are not neccesarry

[G Caputo]

This place rocks! Thank you both, gonna tweak in the post a wee bit more and make me some little parts now!