X offset Crown OSP-10U

[dingo0722]

I am trying to set up the x offset on a Okuma Crown. I have the spindle zeroed to the boring bar holder. With the boring bar holders I can enter G00X0.0 and the turret goes to the exact center of the spindle. when I use an OD cutting tool, I turn a boss on a piece of steel, back off only in Z, go to tool data, select the tool, measure the boss with a mic, hit cal, enter the value for the boss in dia, press write. The value is accepted. When I then do a G00X0.0 for that tool, it never stops at the center of the spindle. What am I doing wrong here?

[underthetire]

You must activate the tool offset in MDI, or program first.

[dingo0722]

Here is the proceedure I am using

\Section 4 - HOW TO SET AN X-AXIS TOOL OFFSET
1. In MANUAL Mode, index the turret to the tool to be offset.
2. Push the TOOL DATA mode button.
3. Start the spindle, bring the tool down to the work-piece, and turn a clean diameter of any size.
4. Carefully back the tool off the work-piece in the Z-axis ONLY!!!
5. Shut off the spindle, and measure the diameter that was just turned. Record the data.
6. Press the EXTEND (F8) key until CAL (F3) key appears.
7. Press the CAL (F3) key.
8. Type in the diameter of the part (found in step 5.) and press the WRITE key.
9. Repeat steps 1 through 8 for all tools.
Note:

[dingo0722]

When I turn a boss, I back off in Z only, measure it, go to tool data select the tool number press Cal, Enter value, Press Write. If I enter 1.25 as the value, the offset value will pop up as 0.603.

If I do a G00X0 then go to tool data, enter in the 1.25 value it shows up as -1.25 in the display on the tool offset page. Something is really screwey here. The only tools I can zero are boring bar/drills that are at 0.000

[littlerob]

When I turn a boss, I back off in Z only, measure it, go to tool data select the tool number press Cal, Enter value, Press Write. If I enter 1.25 as the value, the offset value will pop up as 0.603.

If I do a G00X0 then go to tool data, enter in the 1.25 value it shows up as -1.25 in the display on the tool offset page. Something is really screwey here. The only tools I can zero are boring bar/drills that are at 0.000

I guess I am not understanding the terminology (by the way I know what a boss is) but what do you mean "turn a boss"? I picture a boss being a round part extruded from another plane, very doable with live tools, but you are saying "turn".

Also your boring bar offsets should not be zero.

Robert

[dingo0722]

Well I believe I have solved the problem after many hours. I went through an zeroed every offset, both x and Y. After that when I turned a diameter(boss-sorry) say 1.250, measured the value, inputed it into the tool data page, then did a G00X500 followed by a T0101X1.250G00, the machine landed on the correct x location. I really have no idea what was causing the offset trouble.

Why should I not set the boring/drill holders to zero?

[OkumaWiz]

Well I believe I have solved the problem after many hours. I went through an zeroed every offset, both x and Y. After that when I turned a diameter(boss-sorry) say 1.250, measured the value, inputed it into the tool data page, then did a G00X500 followed by a T0101X1.250G00, the machine landed on the correct x location. I really have no idea what was causing the offset trouble.

Why should I not set the boring/drill holders to zero?

Drills should be set to zero. Boring bars have their tool tip off spindle centerline so you should have an offset that is the amount it would take to get the tool tip to position back to centerline.

A G0 move must be made with T command in order for the offset to become effective.

[littlerob]

Why should I not set the boring/drill holders to zero?

I only meant that if you have a bar in a holder and touched off than the "offset" amount would not be zero. On the other hand as O.W. said your drills should be zero, I only pointed it out because it could have been a contributing factor to the problems you were having. Anyway I'm glad everything is going okay.

Robert

[dingo0722]

Yup understool. I was just refering to the bolt on holders onto the turret.
Working great now. Just ran a basic program.

[broby]

The method I use for setting X axis tool offsets is like this...

1. Move the tool into position to take a cut.
2. On the tool data page, move your cursor to the X offset for the desired tool.
3. Extend to show the CAL command.
4. Press CAL 0 then WRITE. Pay no attention to the resulting tool offset... This will be updated later.
5. Start the spindle and manually take your cut.
6. Move the tool away at the end of your measuring cut on both X and Z as required.
7. Stop the spindle and Measure the diameter you just turned.
8. Return to the Tool Data page and Press ADD and enter the Diameter as a NEGATIVE number then press the WRITE key.
9. Tool offset is correct!

Obviously this method allows you to machine a diameter with out having to "carefully" move away from and return to the machined diameter before Calculating the machined diameter.
This works great for setting boring bars as you are winding the tool along the Z axis in the Negative direction and you can then press the X axis selection and continue winding to 'clear' the bore with out letting the tool rub.
Not only that, but you can move the turret back to home position, or well clear of the bore so that you can get in to measure the bore with out having to worry about having the tool at the machined diameter in order to CAL the size.

When setting multiple tools for Z axis I use a dial gauge with a flat end rather than the usual rounded end.
Set the dial gauge so that the spindle of the dial gauge is aligned with the Z axis.
Move your "Zero Set" tool (the one with tool offset for Z=0) up to the dial gauge to a point where you are happy with the contact.
Set your dial gauge to 0 (zero).
On your Zeroset page CAL the machine position as Z0.
Now move each tool up against the dial gauge and CAL the tool offset for Z axis when the tool is at the dial gauge 0 (zero) point.
Since the dial gauge 0 (zero) point is at Z0 calculating the tool offset results in correct offset for each tool on Z.
This is an easy way of obtaining Z offsets with out having to touch against a face. If you "over shoot" all you do is move past the Zero Point on the dial gauge, no damage to a job or anything else.

Hope you can follow this and get it to work for you all.
Cheers
Brian.

[dingo0722]

wow this is very different method than whats in the manual. I will have to give this a try. thanks

[broby]

it was a method that was shown to me many years ago now.
I like it from the point of view that I do not have to worry about keeping the tool in-position to calculate the required offset.

Using MDI you can easily check your tool offset is correct by typing in the following:
G0 Xposn Zposn T090909
Where posn is the desired position required to place the tool at and the T code is made up of Tool offset number, Physical Tool number and Tool Nose Radius Comp number.
For the purposes of offset checking you could use:
G0 Xposn Zposn T0909
After all at this point you are not really interested in "checking" your TNR offset. Just X and Z posn.
Cheers
Brian.