Lathe master tool

Hello, everyone.
When I want to calibrate the lathe tool presetter in Fanuc 0i TD, how can I use the master tool to make it? And I also don't know how to get a master tool with tool offset data?

Your help will be greatly appreciated.

Yingxi

While I don't know Fanuc controls, the basic principles should be the same as my Okuma.

1) First, input a ~typlical~ offset into your master tool's X & Z.
(close to what that tool would normally have in that machine....)

2) Chuck a piece of scrap bar, and set a G54 (or whatever offset you want) to be at the front of the bar.
You can use your turret to get you close, from machine home

3) MDI the tool to a given diameter, and take a cut on the bar.
Measure, and adjust the X offset until it cuts at the diameter you command.

3) Through MDI, command the tool to go to Z0.0 and test face.
Adjust the tool's Z offset until it cuts in Z where it should.

You have now qualified your "Master Tool"

4) Go into Fanuc's "teach your control where the tool probe is" screen, and teach the X+ and Z+ face of the probe. Your manual or Google should get you that info.

5) From there you can do the following:
On a Haas (and probably Fanuc also) you can use a micrometer to measure the probe size, and back calculate where the X- & Z- sides are.

On my Okuma, you will need to use a boring bar, and a LH tool to qualify the X- & Z- sides.

6) Touch off some tools to the probe, and take test cuts to qualify them.

If the measured data, matches your commanded cuts (within a few 0.001's) you should be good to go.
If not, then you will need to adjust the Tool Probe X- & Z- location in the control......

Doug.

I work for Doosan and Dougs method is good for getting the offsets for a master tool. Where it differs is that on a Fanuc control these numbers are stored in parameters.

The parameters are 5015 thru 5018. Write down the original values somewhere. Also, write down the values for the master tool. Then, adjust the parameters by a few hundredths of a MM. These values are permanently METRIC values, whether you are in inch or metric. After making a small adjustment of each parameter, set your master tool. Keep adjusting and setting until your master tool are equal to the numbers you had initially gotten from cutting a part.

The measurement in Z axis is measured from the ground face of the spindle, behind the chuck, usually. Be careful, write everything down.

Paul

doug925 said:

...
4) Go into Fanuc's "teach your control where the tool probe is" screen, and teach the X+ and Z+ face of the probe. Your manual or Google should get you that info.

Click to expand...

That's a sensible procedure.
I'd like to add that on some controls, like my old T2 Mazatrol, you have to enter the probe position and probe size via parameters.

doug925 said:

While I don't know Fanuc controls, the basic principles should be the same as my Okuma.

1) First, input a ~typlical~ offset into your master tool's X & Z.
(close to what that tool would normally have in that machine....)

2) Chuck a piece of scrap bar, and set a G54 (or whatever offset you want) to be at the front of the bar.
You can use your turret to get you close, from machine home

Doug.

Click to expand...

Hello, Doug
How can I set a G54 when I just input approximate (typical) offset into master tool's X/Z axis?

Yingxi said:

Hello, Doug
How can I set a G54 when I just input approximate (typical) offset into master tool's X/Z axis?

Click to expand...

G54 is just a point in space, to your machine. It doesn't care if it was set by a tool or not.
This is what I do:

1) I assign a G54 2.00" in front of my chuck face. (Tape measure from Turret face @ machine home, to the face of the chuck)

2) Using MDI, command the tool to go to G54. MAKE SURE that your tool is WELL BEYOND the chuck in "X" PRIOR to cycle start!!!

3) Grab a 123 block, tool height gage, or whatever, and adjust the tool in Z until you reach EXACTLY 2.00" away from the chuck face.

4) Adjust the Z offset by whatever amount you needed to move the tool.

5) Have a beer!

Cheers,

Doug.

doug925 said:

G54 is just a point in space, to your machine. It doesn't care if it was set by a tool or not.

Doug.

Click to expand...

But I think G54 should shift the machine zero point onto the front face of the workpiece. In this way, the tool offset can shift the characteristic point of the slide (or turret) onto the tool tip.