Mori Seiki MV45 Yasnac MX1 Help Please

[premier_industr]

Can anyone here please explain how to set work coorinadinants on this control ?

It has been kicking my ass for the last few days.

We bought this machine used with no manuals "yet".

I'm familiar with the Fanuc style programming using G54-G59 and I would like to stay with this format but I am not sure if the MX1 control supports it.

I think that at the time the machine was built it was an option and I am not positive that it is on the machine.

From what I can tell, you can load coordinants into the machine parameters #6516 etc. to tell the machine G54-G59 etc values.

What values do you load ? ( machine position values ? )

But how else would you tell the machine where the part is ?

G92 ? I'm not familiar with this code and have heard alot of bad things about it.

Please help.
Thank you.

[tobyaxis]

Originally Posted by premier_industr Can anyone here please explain how to set work coorinadinants on this control ? It has been kicking my ass for the last few days. We bought this machine used with no manuals "yet". I'm familiar with the Fanuc style programming using G54-G59 and I would like to stay with this format but I am not sure if the MX1 control supports it. I think that at the time the machine was built it was an option and I am not positive that it is on the machine. From what I can tell, you can load coordinants into the machine parameters #6516 etc. to tell the machine G54-G59 etc values. What values do you load ? ( machine position values ? ) But how else would you tell the machine where the part is ? G92 ? I'm not familiar with this code and have heard alot of bad things about it. Please help. Thank you.

Ok I had to do some digging and found my setup information on an MX2 that should be close to what you have.

First thing first. Write a Program that will send the Machine Home at Morning Startup

O0099
(MATSUURA YASNAC MX2)
(SEND MATSUURA CNC HOME)
(SET RAPID AT 25 PERCENT)
(PRESS CYCLE START)
(AFTER HOME POSITION)
(G92 X0 Y0 Z0 IS SET)
(CHECK POINT G55 CENTER)
(RE-CHECK BACK HOME)
(RUNS WARMUP PGM)
(RUN ONE TIME)

G0G17G40G49G80G90M5

G91G28Z0M9
G91G28Y0
G91G28X0

G92X0Y0Z0

G90G55G0X0Y0

G91G28Z0
G91G28X0
G91G28Y0

M98P9999

M30



Next to set G54-G59 you go to the SETTING Page Hard Button.

Edge find your part and Insert The Machine Position Page Numbers Without Decimals.

G54 X=#6516 Y=#6517 Z=#6518 A=#6519

ex #6516 = -10.5000 inches = enter -105000
ex #6517 = -5.6743 inches = enter -56743
ex #6518 = -17.5678 inches = enter -175678

G55 X=#6522 Y=#6523 Z=#6524 A=#6525
G56 X=#6528 Y=#6529 Z=#6530 A=#6531
G57 X=#6534 Y=#6535 Z=#6536 A=#6537
G58 X=#6540 Y=#6541 Z=#6542 A=#6543
G59 X=#6546 Y=#6547 Z=#6548 A=#6549

To set G92 instead of G54-G59 you will input the XYZ Values of the Part Location from the Machine Position Page. These numbers will be in the begining of your NC Program like this

G0G17G40G49G80G98M5
G91G28Z0M9
G92X-10.5Y5.6743Z-17.5678M19

N1(TOOL DISCRIPTION)
T1M6
S5500M3
G90G43G0X0Y0Z1.0H1
Z.1M8
G1Z-1.0F25.0
G13I?J?K?Q?D?F?
G0Z.1M9

G0G40G80G98
G91G28Z0M19
G49

You can also get more information from the Yasnac Site in PDF Files.

http://www.yaskawa.com/site/Support....neSupport.html

Cheers

[premier_industr]

That was my problem.

After referancing out the machine I should have been typing in G92 X0 Y0.

Also found that after refing the machine, type in G52 X0 Y0.

Pretty much the same code as the G92 but different.


My next question, how do you start writing a new program into memmory ?

For instance, on a Fanuc, in edit mode, type O1234 ( prg # ) and then ; ( EOB ) that gives you a new program to start writhing in.

How do you do this on a Yasnac ?

Thanks for all your help on the previous post.
With out you help I would have gone nuts.

[tobyaxis]

Originally Posted by premier_industr That was my problem. After referancing out the machine I should have been typing in G92 X0 Y0. Also found that after refing the machine, type in G52 X0 Y0. Pretty much the same code as the G92 but different. My next question, how do you start writing a new program into memmory ? For instance, on a Fanuc, in edit mode, type O1234 ( prg # ) and then ; ( EOB ) that gives you a new program to start writhing in. How do you do this on a Yasnac ? Thanks for all your help on the previous post. With out you help I would have gone nuts.

Nuts???? That is the definition of being a Machinist, LOL. We have to be NUTS to be doing this for a living

I'll really have to dig for that one. I used to write all my stuff with BCC V19 then use the RS232C Communications.

BRB with some information for you.

[tobyaxis]

Ok this might be it.

EDT (Edit Mode Select Switch)
Prog (Program Key)
Letter "O" the Program #
then the WR (WRITE) Key

That should do it for you.

You might have some other functions as well like G12/G13 Spiral/Helical Interpolation. Good for Milling Large Circular Pockets and Thread Milling.

You have more Drilling Canned Cycles than a Fanuc too. These are Great if your Hand Coding

Hole Pattern Cycles are as follows

G70-Bolt Hole Circle

G70 X? Y? I? J? L?

XY- Positions are the Bolt Hole Center
I- is the radius of the Bolt Circle
J- the degree with the X axis within .001 of a degree accuracy
L- the number of division of the Circumference CCW sequence positive numbers are programmed and vise versa

Ex. of a 6 inch Bolt Circle 1/4-20 Tapped holes

G83G99Z-.5R.1Q.2F5.5L0
G70X0Y0I3.0J60.0L6

G71-Arc Hole Pattern

G71 X? Y? I? J? K? L?

XY- the Arc Center Position
I-Radius of the Arc Programmed with an accuracy of the least programmable increment.
J-the Angular Position of the First hole.
K-Angular spacing in degrees with .001 degree accuracy. Positive values are CCW and vise versa.
L- number of holes to be set in positive numbers

Ex.

G83G99G90Z-.5R.1Q.2F5.5
G71X0Y0I3.0J20.0K20L7

G0G80G98M5
G0G40M9T2
G91G28Z0M19
M6

G72-Line at Angle Pattern

G72 X? Y? I? J? L?

XY-Coordinates of the start point (first hole)
I-Interval is programmed in degrees within an accuracy of the least input increment
J-Angles programmed in degrees with an accuracy of .001
L-Number of hole to be drilled

Ex.

G83G99Z-.5R.1Q.2F5.5
G72X1.Y1.I1.0J15.0L5


You will have lots of fun with this machine.

I have a question for you. Is this Machine a Matsuura?

[premier_industr]

O4321 then the WRite key ( slap my forehead )

That makes plenty of sense I was typing O4321 and then alter or insert.
( that is what you would do on a Fanuc )
Obviously I wasn't having any luck.

You have been a tremendous help and I appreciate you helping me out.

One other quick question for you.

Is there any way, that when you are running a program you can get a split screenthat shows the program being run plus the machine locations / distance to go etc ?

By the way this machine is a Mori Seiki MV45.
Here is a machine similar to it listed on E-bay.

http://cgi.ebay.com/MORI-SEIKI-MV-35...QQcmdZViewItem

This machine is built like a tank !!

[tobyaxis]

Boxed Ways !!!!!!!! You'll take some nice AGRESSIVE CUTS WITH THAT

As far as I know there isn't a Split Screen. Sad that that is the Only Blunder in the entire Control.

You have a PM