[nathanokkema]

I am running and Okuma Cadet LN8C and have mistakenly changed the machines X 0. I am wondering if anyone knows a way to reset the X 0 to where it was before or knows how to get the X0 where it's supposed to be. Prior to changing the X 0 my actual position read 11.9754 and after the change the actual position is at 945.4265.

[Algirdas]

Change actual position doesn't mean your x reference is changed. Bear in mind, the tool offset is calculated in the work point coordinates.
Cut diameter 20 and diameter 50 with "wrong" setting. Take measurement what you have got. Draw a sketch and you will see where machine thinks it's X zero is sitting right now

[nathanokkema]

I was in the Zero set menu when I clicked: Set, 0, Write, and now my X axis is completely off of what it used to be. When I give the machine a homing command G0 X30, alarm B minus var. limit over X axis 1 shows up on the screen.

[Algirdas]

here is how to fix. Check if you have a tool with proven X offset. Lets say it is T05.
Move the turret in safe position. Place the positioning override knobs to minimum.
MDI mode > T0505 <write> M06 <write>
Tool 05 is in the turret with it's offsets
G91G00Z0X0 < write> now the turet can move a little bit but not necessary. Let it move checking the remaining distance and operating he positioning override knob.
chech if target is reached. Means remaining travel both Z and X are 0
Now set the MDI Manual mode and place the tip of the tool ( presuming it is the work point ) at the center of rotation. This will be not precise, butt good for the beginning, so allign the tool tip to center.
Go to zero settings, select X and CALC 0
Move your turrret to safe position. Now you can reset or change mode to manuala or whatever.
This is approximate setting. To find the correct one you need to cut and measure two diameters - for instance 50mm and 5 mm and make a drawing with results. The fine correction will be clear on the drawing.

[broby]

ALL the Lathes I have used have all had their X0 set to the centreline of the ID Toolholder pots.
i.e. Drills have a X0 tool offset, Z offset is as required (Difference between your Z0 tool and the tip of the Drill on Z)
My procedure is thus:
1. Mount your Finger Dial in the Chuck, DO NOT just magnetise the base onto the chuck face as the dial could move around. I made up a bar with a hole drilled in the end face at a similar radius to the hole of the ID holder, screw tapped in from the side to secure the dial gauge.
2. Bring your tool holder down to the dial gauge. Clear of the dial on Z.
3. Roughly align on X by manually rotating the chuck and watching the tip of the finger dial for alignment on the hole.
4. Once reasonably close, Position the tip of the Finger Dial inside the ID Holder and rotate the chuck.
5. Observe the deflection on the dial and move X until you get Zero-Zero from side to side.
While you are doing this, make sure your tool holder is also aligned "Vertically" i.e. not above or below the centreline of the chuck.
If the holder is out Vertically, you will need to adjust the postion (doweled with an adjustable dowel that you rotate to achieve this)
Make sure your holder is also LEVEL along Z, don't just "rotate" to get the front of the ID on Centre otherwise your drills and boring bars will point up or down a lot, depennding on length.
6. Once you have "Dialed" Zero all around, Goto your Zeroset page and Calc X0.

WRITE DOWN YOUR ZEROSET VALUE AND KEEP IT SAFE.

A fast way to get your tool offset set for X is to do the following:
1. Position your tool to take a cut. ID or OD, this method works for both.
2. On the Tool Data page, Select your tool number and CALC X0
3. Machine your material and move the tool away from the part to anywhere you want.
4. Measure your part to your required level of accuracy.
5. Go to your Tool Data page and select the tool number you have used to cut the part.
6. With the X value selected, Add - diameter measured (ie if you measured 2.5045" press ADD -2.5045)
Your tool offset will now be correct for X

To check you have done this correctly, use MDI to move your tool to the measured diameter and visually look, does the tool look like it is in the correct position or not?
i.e.
G00 X2.5045 Z (clear of the end of the part) T0505 (if you are using Tool 5 subs for the tool number used)

Hope you can follow my instructions.
Using this method you do not have to move the tool back to the same position you cut at and then CALC the measured diameter.
Cheers
Brian.

[OkumaWiz]

A quick tip: Your X Zero Set is recorded on the Management Data Card in the electrical cabinet of the machine. If it is there,(a lot of people think they are helping when the remove it for safe keeping) enter the number and verify that the PR Zero Offset number for X is the same as well.
If you are off slightly, use Broby's procedure to correct the X zero point and use the PR Zero Offset number to shift the encoder position. That way all your Stroke End limits, Zero Points, Variable limits all stay the same.That is what you want if you've entered any zero points into a program.

Best regards,