Fanuc 10T Geometry Lock

coulombejerome · Aug 3, 2014

I would like to know if there is any parameter or 'key lock' for the Geometry Offset on a Fanuc 10T.

It's on a Kitako V-turn lathe.

It's right 'No Options' at the Geometry Offset Table.

Thank you !

ImageUploadedByTapatalk1407114940.591339.jpg

Vancbiker · Aug 3, 2014

The Geometry Offset feature is an option. Yes, there is a procedure to unlock it. It's fairly involved and unless you have pretty good experience in servicing CNC controls, I'd advise you order it from Fanuc or look for experienced assistance.

coulombejerome · Aug 4, 2014

Ok ... What are my other options ? I only have a Wear tools offset table avalaible. When i put a value in it, the program stop at the changing tool line (t0808 for example) . Even if it's a smaĺl or big value.

Do you have an idea ? Is there an another place to put tools offset ?

Than you !

ImageUploadedByTapatalk1407150395.906729.jpg

coulombejerome · Aug 4, 2014

I found this page in the Operator's programming manual. Is anybody familiar with this procedure ?

Thank you !

ImageUploadedByTapatalk1407156931.608441.jpg

Do I enter these commands for each tools ?

yardbird · Aug 4, 2014

I wouldn't have thought so but maybe your machine is set up to use G50's. The picture in you last post looks like the T or tool tip in your wear offset page In post 3. It is what point of the tool that is programed. Do you have a work shift offset page at the machine?

Brent

angelw · Aug 4, 2014

coulombejerome said:
Ok ... What are my other options ? I only have a Wear tools offset table avalaible. When i put a value in it, the program stop at the changing tool line (t0808 for example) . Even if it's a smaĺl or big value.

Do you have an idea ? Is there an another place to put tools offset ?

Than you !View attachment 113600

Include G00 in the same Block as the Tool Call as follows:

G00 T0808

If this lets you program progress, as I expect it will, you can modify a parameter to change the way in which the Offset is applied. Post back with the result of including G00 in the Tool Call Block.

Not too many FS10 controls were supplied without the Tool Geometry Option. I suspect that the parameters may have been lost at some stage and the Option Parameters not reinstated. If you're lucky enough to have the Fanuc Control Specification sheet, the Options supplied with the control will be listed there. Alternatively, contact the Machine Builder, quoting the machine's serial number, and they will be able to tell you what Options were supplied. If the control came with the Tool Geometry Option, you should be able to get it reinstated for the cost of a Fanuc service call.

Regards,

Bill

coulombejerome · Aug 4, 2014

yardbird said:
I wouldn't have thought so but maybe your machine is set up to use G50's. The picture in you last post looks like the T or tool tip in your wear offset page In post 3. It is what point of the tool that is programed. Do you have a work shift offset page at the machine?

Brent

Yes I have. Here is the picture :

ImageUploadedByTapatalk1407166095.969149.jpg

yardbird · Aug 4, 2014

The best advice I can offer now is do as instructed by the fella in post #6 he is by far more knowledgeable than I. Im betting a parameter got lost in your control. Did you try G00 T0808? You might put a offset in the tool your calling and notice if the machine moves by the offset amount. That should tell you how your machine applies offsets. Weather its on the T call or the next G00 move.

Brent

coulombejerome · Aug 5, 2014

I put a G00 in front of my T0808 and it work ! ... The tool change and the value I enter in the Wear Offset Table are good!
So, I have to enter the offset value in the wear offset table and put G00 in front of all my toolchange commands. Is this sound logicial or it's the first time that you see that?
The Geometry Offset Table with no options is weird ... but ... if it work with the wear offset that's good.

Thank you all for your help !!!

angelw · Aug 5, 2014

coulombejerome said:
I put a G00 in front of my T0808 and it work ! ... The tool change and the value I enter in the Wear Offset Table are good!
So, I have to enter the offset value in the wear offset table and put G00 in front of all my toolchange commands. Is this sound logicial or it's the first time that you see that?
The Geometry Offset Table with no options is weird ... but ... if it work with the wear offset that's good.

Thank you all for your help !!!

With regards to needing the G00, its quite typical but parameter related. Its a parameter I don't visit often with a FS10 control, so I've not committed it to memory. I'll look it up when I get a chance. The other thing you need to be wary of, is that the slides don't move during the Tool Change Operation, if the Tool Offset is called at the same time and without a move command. In this case, the better Format for your program is as follows:

G50 S 3000 T0100 (SELECT THE TOOL WITHOUT OFFSET)
G96 S_ _ _ M03
G00 X_ _ Z_ _ T0101 M08 (APPLY OFFSET DURING MOVE BLOCK)

If the slides don't move during the following command:

G00 T1010

Then you can just select the Tool and Offset as shown immediately above.

Its possible for one of the following "G" codes from Group 1 to be modal:

G00, G01, G02, G03

The G02, and G03 are very much less likely, as you would have had to have stopped a running program during, or immediately after a Circular Interpolation move. Accordingly, it's much more likely that the Modal Group 1 "G" code will be G00, or G01. When the control is initially turned on, G00 will be Modal as the default setting, but it can be changed via parameter.

You would have found that had the Spindle been running, and a Feed Rate specified, that the program would have made it past the Tool Change Operation without the need to specify G00 with the Tool Call. This is a hangover from very early controls, but is a Format I still use and write into CAM Posts. By specifying G00 with the Tool Call command, you're sure of the Group 1 "G" code that is modal.

Regards,

Bill

coulombejerome · Aug 7, 2014

angelw said:
With regards to needing the G00, its quite typical but parameter related. Its a parameter I don't visit often with a FS10 control, so I've not committed it to memory. I'll look it up when I get a chance. The other thing you need to be wary of, is that the slides don't move during the Tool Change Operation, if the Tool Offset is called at the same time and without a move command. In this case, the better Format for your program is as follows:

G50 S 3000 T0100 (SELECT THE TOOL WITHOUT OFFSET)
G96 S_ _ _ M03
G00 X_ _ Z_ _ T0101 M08 (APPLY OFFSET DURING MOVE BLOCK)

If the slides don't move during the following command:

G00 T1010

Then you can just select the Tool and Offset as shown immediately above.

Its possible for one of the following "G" codes from Group 1 to be modal:

G00, G01, G02, G03

The G02, and G03 are very much less likely, as you would have had to have stopped a running program during, or immediately after a Circular Interpolation move. Accordingly, it's much more likely that the Modal Group 1 "G" code will be G00, or G01. When the control is initially turned on, G00 will be Modal as the default setting, but it can be changed via parameter.

You would have found that had the Spindle been running, and a Feed Rate specified, that the program would have made it past the Tool Change Operation without the need to specify G00 with the Tool Call. This is a hangover from very early controls, but is a Format I still use and write into CAM Posts. By specifying G00 with the Tool Call command, you're sure of the Group 1 "G" code that is modal.

Regards,

Bill

Yes the slides moves ... so I did what you said. Call the tool without offset than call the offsets during the next move. It works great!

But I have another problems ...

When I go to the home position (G28 U0. W0.) I want it to remove the offsets during the move to be ready to call another tools (same as you told me before). If I call the tool without offset (T0100) at the home position, It go Overtravel (depending with which tools ...)

So , with
G28 U0. W0. T0100;
It will first do the offset and then move back to the home position.

Do you have any idea to do the offset DURING the move to the home position ...?

Thank you!

coulombejerome · Aug 8, 2014

I just put a G40 on the G28 U0. W0. line and it work but ...

G20 G18 G40;
G97 S200 M03;
G00 T0800;
G0 G54 X2.5 Z0.5 T0808;
G40 G28 U0. W0.;
G18;
G97 S250 M03;
G00 T0700;
G0 G54 X2.5 Z0.5 T0707;
G40 G28 U0. W0.;
G18;
G97 S300 M03;
G00 T0100;
G0 G54 X2.5 Z0.5 T0101;
G40 G28 U0. W0.;

The only problem is :

At the line G00 T0700;

The position BEFORE the Toolchange is x0 z0 machine.

After the tool change it's x0.5822 z0.0017 which is the Offset of the Tool 8 (First tool of the program)

The slide move during the Tool change ... ONLY at the second toolchange of the program. It looks like the Offset of the first tool has not canceled.

Someone know how to do that ?

Thank you!

Search

Largest Manufacturing Technology Community on the Web

Search

Fanuc 10T Geometry Lock

coulombejerome

Plastic

Vancbiker

Diamond

coulombejerome

Plastic

coulombejerome

Plastic

yardbird

Titanium

angelw

Diamond

coulombejerome

Plastic

yardbird

Titanium

coulombejerome

Plastic

angelw

Diamond

coulombejerome

Plastic

coulombejerome

Plastic

Similar threads