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.

[Eurisko]

Hi,

I have experience with a Mori MV-40 with a Yasnac control.

Our control provides only 3 different work offsets, G54 G55 G56.

Coordinate values can be preset by the program or input manually by repeatedly pressing the "Settings" button until the work offsets page is displayed.

Use the absolute/relative toggle button to switch between INPUT/INPUT+ (Fanuc style). Cursor to the desired offset/axis, type the new coordinate value and press WRITE (Enter).

It's easier to DO than describe


To change these values through the program:

We'll input the coordinate values X+1.0000 Y-2.0000 Z-3.000 into G54.
Here's the block of program code:

N1 G10 L2 P1 X+1.0000 Y-2.0000 Z-3.0000

(Note: The 'P1' in line N1 references G54.
Substituting P2 would reference G55, P3 would reference G56.)

Now, we'll make G54 active and rapid to our new zero point

N2 G90 G00 G54 X0 Y0


All work offsets are referenced from machine zero.

Hope this helps...

[premier_industr]

I thinkI got it to work, pretty much like you described.

The only thing I had to do before trying to run the program is send the machine to the G53 X0Y0 and type in G52, then start the program using G54.
The program would continue to run just fine after this.

This is the only way that I could get the machine to load the G54-G59 values.

Is this right ?

I have not tried the G10 code but I think that I will also give this a shot.

Thanks for the help !!

[Eurisko]

Glad to help.

Our controller is a Yasnac I80M, wasn't sure about that when I posted last night.

When using the program to set the work offset, you may have to put a G90 before the G10 (on the same line) .

I have NO idea why the G53 / G52 codes are needed on your control, but if it works, go for it. Probably resets the work coordinate system to the default condition.

Yasnac controls sometimes behave strangely. Such as jumping to a random spot in the program when the reset button is pressed. Not every time, just sometimes.

Makes it interesting when rerunning a tool.

[premier_industr]

Do you usuall y use the G10 code to load the offsets ??

Or do you type them into the parameters manually ??

Your previous answer brings up another question I have.

This control will not let me start a program unless it is from the very begining.

For instance, I have a 2 tool job, spot drill and then drill.

If I spot all the holes and then make a tool change to the drill, hit reset, check hole locations ect. It will not let me start at that point in the program.

I get an alarm something like "reset is not correct".

After hitting reset and scrolling back down to the drill portion of the program, hit cycle start, same alarm.

WHY ??

[Eurisko]

Do you usually use the G10 code to load the offsets ??

This machine uses a touchsetter to establish the work offset. The machined part has to be concentric within .004 TIR from the previous lathe operation.
The G10 code sets the work offset close enough for the touchsetter to find the bore. The touchsetter routines then 'tweak' the offset, usually within .001 TIR.

On rare occasions when the touchsetter isn't used I manually zero the fixture using the work coordinates screen.

This control will not let me start a program unless it is from the very begining. For instance, I have a 2 tool job, spot drill and then drill. If I spot all the holes and then make a tool change to the drill, hit reset, check hole locations ect. It will not let me start at that point in the program. I get an alarm something like "reset is not correct". After hitting reset and scrolling back down to the drill portion of the program, hit cycle start, same alarm. WHY ??

That's a tough one to answer. All of the Fanuc controls I've seen (& the Yasnac) operate similarly. Very easy to start from ANY point in the program.
Unfortunately, a reset will set the control to a default state. It's hard to determine what the 'default' state is without documentation. If a tool is cycled after a reset, you can't assume that your cutting parameters haven't changed.

We use 'safe start' lines for each tool. These lines of code initialize the control to a known state ( inch system, xy plane selection, work offset, etc) before the tool is used. In your case, you may have to copy the initialization code at the beginning of the program and paste it at these 'safe start' points.

Personally, when rerunning a tool, I press the 'EDIT' button, page down or cursor down to the safe start line, then press 'EDIT' again to go into 'AUTO" mode. I press reset, make sure that the control hasn't randomly jumped to the wrong line, then 'CYCLE START' .

If your control has a 'mid-auto manual' feature ( Okumas do ), you can interrupt the program, jog the table, move the spindle, etc., and continue on with a press of the 'sequence restart' button. Very handy.

I wish I could be more help! These controls really require the 'hands on, trial-and-error' approach. There are many ways of getting the job done, even if you have to use subroutines or GOTO blocks to jump around.

Your machine wouldn't happen to be in Ohio or Michigan, would it? It sounds like a challenge...

[danohpsp]

I have and MX1 and two Yasnac 3000G's.

The MX1 does have the G54-G59 command. With this, you just put the coordinates of the fixture in particular parameters in the machine. Once the coordinates are entered in the parameters, when you use G54 or similar, the machine switches to the new coordinate system.

You can also use the G92 code, which I think is easier. On the Yasnac 3000G's you do not have the G54-G59 codes available so you must do it this way. I normally start my programs like the following:

G17G40G80G90G49G98
(this is just some setup stuff)
/G91G28X0Y0
(go in incremental mode so that a motion does not occur before return to zero G28 is issued, then go back to the machine's zero in X and Y)
/G91G0X-10Y-3 (run to the zero of the fixture. Here we assume that X-10 and Y-3 is where the fixture is.)
/G92X0Y0 (once you are at the fixture location, use G92 to make this the new zero point, similar to doing an ORG)
G90 (go back into absolute mode)

The / command is in front of these codes is in order to allow you to not have to run back to the machine home every time you press start to run a new part. If you flick up the block skip switch on the machine, the machine will just skip this zero fixture point setup on the next run, since it is already positioned on the new coordinate system. Be very careful in the rest of your code if you use this block skip feature, especially if you stop the machine mid-cycle and manually ORG something out. It does not hurt as a safety feature to run to leave the block skip off and run to home every time especially if the program is large or being drip-fed. If you forget to flip off the block skip feature at first power up of the machine, most likely you will hit an axis limit on your first run of the program.

By the way, on the 3000G's, don't include comments in the code because the control does not support comments. Otherwise these are all good easy to use controls.

Hope this helps. By the way, Yasnac manuals for the old controls are available from Yaskawa's website at www.yaskawa.com