Mazak Dynamic work offset problem.

[rsbeadle]

I have moved to a shop that has several Variaxis machines. We are not able to use the Dynamic work offset feature because our parts are too high above the center of rotation. Every time the machine reads the G54.2P1 it makes an incremental move that is the amount in the x, y, and z axis fixture offset. We use G54.1P1 as the center of rotation, move to a point off the part by hand editing the code, and let it make the incremental move it wants to make. The problem is on larger parts there is not enough room to clear the Z move without hitting the part. Is there a parameter in the machine or a work around that can keep the machine from making the move when it reads the G54.2P1? When our tool is 8" gage length and the part is more than say 5" above center of rotation, the tool has to go lower than the face of the part to allow for G54.2P1 to move up the 4" that is in the fixture offset in Z.

 

G54.1P1 center of rotation value is:

 

x-10.03937

y-7.28364

z-20.07874

 

G54.2P1 fixture offset value is:

 

x-.5000

y+.5000

z+4.0000

 

We have to hand edit the g0g90g54.1p1 line to make z drop down 4" from home position to allow it to go back up 4" when the machine reads the G54.2P1 or it soft limits the machine. We have to allow for the tool length also.

 

Any help is appreciated. If you need more info just let me know. Thanks.

[crazy^millman]

I would add a mi or mr to the post that allows you to decide if you want to use. Might need to add the tool length to the tool parameter page if you want the length to be used. Then activate the mi or mr and then in the pretract part of the post have it look for the mi or mr and then use the code you have above pull a value from the toollength variable to add to what you need and then done.

 

HTH

[robk]

We use dynamic comp on our Variaxis' and we do not have that problem.

Do you mind posting a sample of your code?

[rsbeadle]

I can send a sample of the code if you still need it, but the only code that is a problem is the G54.2P1. Every time the machine reads G54.2P1 it makes the incremental move in the amount of the G54.2P1 work offset numbers. If there in not a G00 or G01 with a feed rate the machine alarms with a feedrete 0. G90 or G91 active does not make any difference. I am sure it is a parameter problem, but all 7 of our Matrix Variax machines have the same problem. I have tried every sample program variation I could find from this forum and others and the same thing always happens. I even tried having Mazak send us a test program and we get the same result. I have went thru the parameter books and tried changing any parameter that has to do with dynamic offset. I found one parameter that keeps the G54.2P0 from making a move but it did not stop the G54.2P1 from moving. We have renishaw probes on all the machines if that may be causing any problems. My predacessor said he had worked with Mazak Applications with no luck, but I haven't tried them yet. They are my next try if nobody here has had to solve this problem before. Again any help is appreciated.

[Jeremy Herron@DBS Solutions™]

We have several Variaxis 730's with matrix controllers and the inhouse post, and to my knowledge there is no way to keep the machine from moving when it calls g54.2 p1 only when you cancel can the move be avoided. Here is sample of my code at it works fine for me everytime:

 

 

G10 G90 L21 P1 X[#5521] Y[#5522] Z[#5523] A[#5524] C[#5525]

G00 G17 G20 G40 G49 G80 G90

G54.2 P0 G53 Z0.

G91 G28 Z0.

G28 Y0.

G30 X0.

M43 (C-AXIS UNLOCK)

M46 (A-AXIS UNLOCK)

G28 A0. C0.

N1(TOOLPLANE NAME - FRONT)

T1 M06 ( 11/32 GUHRING DRILL)

G91 G28 Z0.

(MAX - Z19.)

(MIN - Z17.177)

G59-----------------(my center of rotation stays in g59)

G00 G90 A-90. C180.

M44 (C-AXIS LOCK)

M47 (A-AXIS LOCK)

M131

G17 X-12. Y12. S1665 M03 ---------------(I have mr7 and mr8 to establish my initial x and y before g54.2 is called)

Z18. ---------------(I have mr9 to establish my initial z before g54.2 or g43 is called)

G54.2 P1

X0. Y.133

G43 H1 Z19.

G94

G98 G81 Z17.177 R17.377 F5.

G80

M09

M05

G54.2 P0 G53 Z0.

G91 G00 G28 Z0.

G28 Y0.

G30 X0.

M43 (C-AXIS UNLOCK)

M46 (A-AXIS UNLOCK)

G28 A0. C0.

M44 (C-AXIS LOCK)

M47 (A-AXIS LOCK)

G90

M30

 

 

I just have to make sure that I set mr7,mr8, amd mr9 far enough away from toolchange position and clear of the part to allow for the move for the amount of dynamic offset I have.

 

If you truly do not have enough room to make this move. You could program off center of rotation and just use your dynamic offsets for the small amount you might be off from your set-up thus making these numbers and the move as small as possible.

 

Hope this helps.

 

let me know if you have more questions.

[rsbeadle]

Thanks for the help guys. I will try some things and get back to you and let you know how it goes.

[Brewster]

i know this is a little late but there is a parameter to turn off the movement. we have a variaxis in our shop and we have turned it off. not sure of the exact one but i believe it is F87, check your parameter books

[torianmachineworks]

i know this is an old thread but was anyone ever able to resolve this issue. i am having the same problem. also, what does the f87 paramter control?

[jlw™]

Are you getting an overtravel alarm?

[jhyp]

On 12/13/2017 at 4:36 PM, torianmachineworks said:

i know this is an old thread but was anyone ever able to resolve this issue. i am having the same problem. also, what does the f87 paramter control?

F87 Bit0 is to offset the tool in the deviation vector, according to the manual, I'm not sure if that means it will turn off the movement if you turn it off, or what. I never had this problem and it seems to may be eliminated by programming slightly differntly.

 

If you have G54.2 P1 on its own line it will move the amount in X Y Z of your dynamic offset. If you put G54.2 P1 Xx yY Zz on the same line the machine will move to those points directly (at least when I've used it)

 

So if you have G54.2  (In your offset page)

P1

X0.0

Y5.0

Z5.0 

 

Then code out

G54.2 P1(ON THIS LINE THE MACHINE WILL MOVE X0.0 Y5.0 Z5.0)

X0.0 Y0.0 Z2.0(THE MACHINE WILL THEN MOVE HERE)

Z0.0 (move down to z from 2 inch safety move)

 

If you code this way

g54.2 P1 X0.0 Y0.0 Z2.0 (THE MACHINE WILL MOVE HERE DIRECTLY)

Z0.0 (move down to z from 2 inch safety move)

[huskermcdoogle]

This goes along the lines of if you should apply g43.4 before or with your first position move.  It all just depends.  But I am a firm believer that if you can get predicatble movement by applying with the move, that's what you should do.  In my case with g43.4 the behavior is somewhat unpredictable as to where the tool tip will end up in path if you do it with, however the cycle time is faster...  So if it clears let it fly....  But if you need to keep control of the tcp, you do it before...

I'm curious to see how this works out. I have never used G54.2, but would like to understand it a bit better.