[jake_tb]

Hi Guys

I am creating a macro to offset the coordinate system based on a table rotation. The machine is a MA-60 horizontal machining centre with a OSP-U100M controller on it, it has a 4th axis table that rotates around Y.
We have a Doosan machine with a fanuc 31i that we have created a Dynamic offset function on and it works so well we want to do the same on our Okumas.
What we have done is setup a macro that you call as follows:

G123 D1 R90 (D=coordinate offset number, R=table rotation)

This will take the current work offset (any number between 1-47) and rotate about the true centre of table by the value specified as "R". The macro uses trig to work out where the new datum X0, Y0 is relative to the old one and then moves the datum by that amount so you only need to setup one coordinate system no matter how many offsets you are using on the job and all the programmed values can stay in absolute mode!

Does anyone use a similar system that can help as I am not as familiar with the Okuma variable address!

[Superman]

Okuma has already a "Fixture Offset Function" that is accessed thru a call statement

ie

[For C/A axes]
CALL OO88 (PX=___) (PY=___) (PZ=___) PC=___ PA=___ PH=___ (PP=___)
PX, PY, PZ: Parallel travel from the reference work coordinate
system (PH) when A = 0, C = 0
Default: 0
PA, PC: Rotational travel from the reference work coordinate
system (PH) when A = 0, C = 0
Not omissible
PH: Reference work coordinate system No. Not omissible
PP: Offset coordinate system number (zero point which
is always rewritten)
Default: currently selected
coordinate system

I've attached our manual for a 5-axis E100M control to look at

[budgieW]

Okuma Also has this for a horizontal. If your machine has IMAP it is in the control

CALL OG367 PB= PH= PHW=

There is also an Okuma *.SSB file to do this. Your local Okuma tech will have it

[Algirdas]

it looks very complicated and strange at the beginning. Let me guess. You want to repeat the same program at several different coordinates?
So You have a lot (20 or more) user defined zero points.
The command G15 H3 is selection of zero point 3 and so on.
These zero points also can be defined in part program by variables:
VZOFZ, VZOFY and so on

[jake_tb]

Hi guys

Thanks superman and budgie for your reply's, I am looking into how they will work on our machine.

Algirdas, the idea of the offset function is not so much to repeat the same operation (as in multiple parts at different datums) but more for one job that has lots of different angles. If you use the standard setup, every time you rotate the "B" axis (table) you have to setup a new datum to machine the new bit of the same part and you then have to try and tie it up to the original datum. The dynamic offset function allows you to set one datum and then every time you rotate the table, the control works out where the original datum is now. It makes setting up jobs so much quicker and less chance of an error!

Jake

[Algirdas]

Thank You.
Now I understood:
You want control to move selected coordinate zero point regarding B axis indexing (rotation). This makes drawing (model) more simple - single "datum" point.
That's cool. I'll try in my area.

[Darek833]

For some time I have a similar problem. The machine is VH-40 with OSP7000M controller.The machine has a rotary axis (C axis) and tilting axis (B axis)
Is there "Fixture Offset Function" for this machine? I tested the command CALL OO88 (PX=___) (PY=___) (PZ=___) PC=___ PB=___ PH=___ (PP=___) but the controller does not accept name subprogram.

[budgieW]

Yes there is but unlike the newer machines this macro is not in the *.MSb file. You will need to get from Your local Okuma dealer or Okuma europe Germany

[Darek833]

If this is not a file * .MSB, what is the format of this macro? Perhaps this macro is on this machine, but I am user of this machine since 2004, so I do not know the history of this machine. If you can still write format command?

[Darek833]

I am looking for a parameter which we set zero machine (the machine with B and C-axis). I have the 0.4 mm difference in x direction between the machine zero and C-axis rotation center. In this case, does not help correct the pivot distance in x-axis. It is certainly "nullpunkt korrektur" in system parameters (controller in German) (system variable VMOF *= 16...,...), but I am not sure if I can simply correct this parameter.

[Algirdas]

don't be afraid. You can save the parameter and restore it back if needed

[Darek833]

thanks Algirdas, now rotational shift of zero point should be calculated correctly

[headflow]

I am creating a macro to offset the coordinate system based on a table rotation. The machine is a MA-60 horizontal machining centre with a OSP-U100M controller on it, it has a 4th axis table that rotates around Y.
We have a Doosan machine with a fanuc 31i that we have created a Dynamic offset function on and it works so well we want to do the same on our Okumas.
What we have done is setup a macro that you call as follows:

G123 D1 R90 (D=coordinate offset number, R=table rotation)

This will take the current work offset (any number between 1-47) and rotate about the true centre of table by the value specified as "R". The macro uses trig to work out where the new datum X0, Y0 is relative to the old one and then moves the datum by that amount so you only need to setup one coordinate system no matter how many offsets you are using on the job and all the programmed values can stay in absolute mode!

Hi Jake,
I have been looking for that function for my HMC with fanuc 16i, could it be possible to have a look at your macro?

[budgieW]

For a Fanuc

%O9018 (G201 -- XZ COORDINATE ROTATION PROGRAM)
(PARAMETER 6058)
#10=[13980+[#4130*20]](CURRENT FIXTURE OFFSET NUMBER)
#11=[#10+1](NUMBER FOR CURRENT OFFSET X)
#12=[#10+2](NUMBER FOR CURRENT OFFSET Y)
#13=[#10+3](NUMBER FOR CURRENT OFFSET Z)
#14=[#10+4](NUMBER FOR CURRENT OFFSET B)
#15=[ABS[#921]-ABS[#[#13]]](Z LENGTH FROM PALLET CL)
#16=[#[#11]](X LENGTH FROM PALLET CL)
#17=SQRT[[#15*#15]+[#16*#16]](HYPOTENUSE LENGTH)
#18=ATAN[#16]/[#15](ANGLE FROM PALLET CL TO PART ORIGIN)
(NOW MAKING NEW G59 COORDINATES)
#19=[SIN[#18-#2]*[#17]](PART ANGLE + ORIGIN ANGLE X LENGTH)
#20=[COS[#18-#2]*[#17]](PART ANGLE + ORIGIN ANGLE Z LENGTH)
#5321=[#19](X G59 COORDINATE)
#5322=[#[#12]]#5323=[#921]+[#20](Z G59 COORDINATE)
#5324=[#[#14]]
M99%

[headflow]

Thank you BudgieW
I got it all working now..

[vpalfi]

Hello, do you have the solution for offset a coordinate system for Fanuc, B axis ? I can help you for Okuma . Thank you.