Okuma Work Coordinates

[firedog]

I am doing multiple parts on a jig fixture, and using one main work coordinate for the fixture itself. I am using a sub program for the machining of each part, but I need to be able to shift my work coordinate to go to each location. This is on an Okuma OSP700M control. I figured out how to use the sub and rts commands, but don't understand how to make a shift effective.

Thaks in advance!!

[brtlatjgt]

In your zero offsets page, your zero for each location,offset 1,2,3, etc.
in your program to shift to 2nd offset put in g15h2, g15h3, etc.
be sure at end of program to put g15h1 to return to original zero.

[firedog]

I have considered that, but I would rather be able to use the incremental distance instead. If I use G15H1 for the main fixture location, then use an incremental shift, I have to only set the G15H1 each time this is set up. I could then make adjustments to each part by changing the incremental value.

[Mortek]

Does Okuma support G10 Loading different offset numbers for x,y,z ?

[firedog]

Okuma controls do support G10 shifts, but it is an option that we didn't purchase for these machines. I was able to come up with a way to make my shift how I wanted. I am using a variable with a math function as follows:

(G15H1)
VZOFX[1]=4.0
VZOFY[1]=-2.00
VZOFZ[1]=6.4097

(G15H2)
VZOFX[2]=VZOFX[1]-3.00
VZOFY[2]=VZOFY[1]+2.00
VZOFZ[2]=VZOFZ[1]

(G15H3)
VZOFX[3]=VZOFX[1]+3.00
VZOFY[3]=VZOFY[1]+2.00
VZOFZ[3]=VZOFZ[1]

(G15H4)
VZOFX[4]=VZOFX[1]-3.00
VZOFY[4]=VZOFY[1]+4.00
VZOFZ[4]=VZOFZ[1]

(G15H5)
VZOFX[5]=VZOFX[1]+3.00
VZOFY[5]=VZOFY[1]+4.00
VZOFZ[5]=VZOFZ[1]

The first VZOF? statement sets my G15H1 location, and the rest of the statements shift G15H2-G15H5 based from that location. Each statement adds or subtracts from the X or Y value and enters it into the required location. In my program I just call up which ever work coordinate I need for the particular machining I am doing.

[Mortek]

If your subroutine is programed at zero then another way would have been to do absolute movements to your next location, change to incremental run the subroutine, then change back to absolute to move to next location thus not having more workshift offsets involved.

Example:

G15H1 G0X0Y0
X-3.00 Y2.00(1st location)
G91(INCREMENTAL)
M98 SUB
G90 G0 X3.00 Y2.00(second location)
G91
M98 SUB
G90 G0 X-3.00 Y4.00(third location)
ETC.

Changing to incremental lets you run the program wherever you want. The sub just has to be programmed at your zero origin

If you are using a cam system to program then program your subroutine incrementally.

The hardest thing to remember if you program manually is the Z moves. If you step down in cuts you have to remember to raise Z back up the accumulated value of the steps, plus your clearance.

[firedog]

The amount of program for each subroutine is pretty extensive, so I wanted to try and stay in absolute if I could. What I been looking for at first was an incremental shift, similiar to what a fanuc control would use. Waht I came up with will work just as well.
Thanks for all of the input!!

Firedog

[Mortek]

You would still only use the one subroutine for each location just like you are now.