Problem- Part Zeroing - Anybody have a easier method than this

[MMTechi]

Part Zeroing - Anybody have a easier method than this
- I Don't have macros

When trying to find the center of a rectangular part, I use these steps:

1. touch off on the right side, zero DRO,
2. move to the left side and touch off,
I take the distance traveled from the DRO and plug into a hand held calculator, and divide by 2
3. change to work offset page, cursor to x column, select PART/ZERO/SET
capture current location
4. then type in value from my calculator, and write/enter/add value
to x offset, this sets "G54" at center of part

Repeat for y direction

Is there a way to capture the 2 locations and split the difference using any copy or calculate commands in the control?

I think this would be a nice option for setup, split distance-find center like on the simple manual mill digital readouts.

I don't have macros but are there any variables available for a few commands or a simple data gathering commands to do this?

Thanks for any help

[wwendorf]

Most of my parts are designed so that the top left of the part is x0, y0

I use one of the touch probes that are .20" wide. So, when I touch off on the top of the part I then set Y to +.10

I then touch off on the left of the part and set X to -.10

Been working really well for me so far.

Wade

[christinandavid]

On Fanuc I tend to use my 'relative' (or 'operator') co-ordinate system. Set to zero on 1st side then whatever figure I come up with, say 123 on the 2nd side I would then enter '1' '2' '3' '.' '/' '2' '.' I would finally move to zero and set my 'work' offset there. Pretty fool-proof.

Not sure if Haas control would accept this notation.

DP

[colton_m]

There is a way to avoid using a calculator with your current method:

For the X axis,

Edge find the right side of the stock then origin the Operator position. Edge find the left edge of the stock and press part zero set (G54). then simply jog to the right until the numbers in G54 X and Operator X are equal (obviously the signs will differ). This will be in the middle of the stock, press part zero set again and you're done, repeat for the Y axis. Exact same idea as yours just avoids the calculator

[Geof]

You can do it all on the offset page.

Touch your probe off on the + side in X and with the cursor on the X column on a line for a work offset you are not using press Zero Part Set.

Go to the - side and touch the probe off, move the curtsor down one line in the X column and again press Zero Part Set.

Use your calculator to take the average of the two X positions and enter that into the X for the work offset you want to use.

Do the same for Y then just wipe out your entries by entering 0.0 and pressing F1.

This way you do not need to know the diameter of your probe, and if you rotate the spindle 180 degrees between each side so you are using the same location on the probe it does not even need to be running true. And if you are using paper for touching off the probe you don't have to worry about the thickness.

[pld0vr]

I have 1" fixture plates for all of my parts the size of the table. They slide onto dowel pins that I set into the table, and then fasten down with counter sunc allen bolts into 4 t-nuts The zero is always the center of the plate, where I made a center bore in-case I need to pick it up again for some reason, and z-0 is plate surface.

So basically what I am getting at, is that the work offset is always the same no matter what I am making.

Doesn't help for fixture making and one offs, but the way to go for production work.

[Sea_en_see]

I use my Renishaw probe. Simple.