Need Help!- Trying to Ball Pick with live tool on Puma2500LSY mill/turn machine!!!

[nato31]

Please help!!!!!

I'm trying to cut a surface with a 1/16" ball nose end mill, but it's cutting my surface WAY SMALL. I don't know how to get my machine out of Diameter mode and into "Radius" mode. I just want to ballpick a surface just like someone does on a mill machine. It's a Doosan Puma 2500LSY with a Fanuc 31i controller. It has a main and subspindle and X, Y & Z axis.

Any help would be greatly appreciated!!!

[dcoupar]

Sorry... what is "ballpick"? Can you post a picture/drawing of the part and the program? I don't believe you can switch between diameter and radius programming.

[sinha_nsit]

Can try 1006#3 (DIAx) = 0

[nato31]

It's funny because right after I posted my problem yesterday, I found an old post regarding the same problem someone else was having. Anyways, changing parameter 1006 Bit #3 to 0 WORKED!!! I just have to remember to have my operator switch it back when we do turning work.
Thanks a lot for replying. It's nice to have such a big community of fellow manufacturers from which to get help from.

Thanks again!!!

N.B.

[Jonnis]

On my mori seiki nt whit fanuc 31i i have a g code and a m code to swith dia - radius .. but i not remember now what they are..

[angelw]

Originally Posted by nato31 It's funny because right after I posted my problem yesterday, I found an old post regarding the same problem someone else was having. Anyways, changing parameter 1006 Bit #3 to 0 WORKED!!! I just have to remember to have my operator switch it back when we do turning work. Thanks a lot for replying. It's nice to have such a big community of fellow manufacturers from which to get help from. Thanks again!!! N.B.

Rather than rely on memory, the parameter can be changed by including the code for Programmable Parameter Entry via G10 in your part program. If you generate programs using a CAM package, the post can be modified to output the appropriate code depending on how the X value is to be interpreted by the control.

The syntax is as follows:

G10L50 - Parameter entry mode
N1006 R 00001000 - Sets bit 3 of #1006 to 1.
G11 - Parameter entry mode cancel

Note: All other bits not to be altered have to be included in the R address as they are currently set.
Changing the above parameter and various others requires that the machine power be cycled. Changing any of these parameters will generate an error forcing the the power to be cycled before normal operation can be resumed. Accordingly, if the above method is used to alter #1006, the code should be included at the start of the program and Block Delete, or a Macro statement used to avoid the G10 code being exercised during subsequent cycling of the program.

Regards,

Bill

[sinha_nsit]

1006 has other parameter bits also which should remain same in G10 L50.
Hence, one should find out the current setting of all bits of 1006 before overwriting it.
I am not aware of any method which reads the current setting of a parameter inside a program, unless there is a system variable associated with it.

[texaspyro]

Originally Posted by sinha_nsit I am not aware of any method which reads the current setting of a parameter inside a program, unless there is a system variable associated with it.

On some machines you can write variable #6998 with the number of the parameter you want to access. Then read/write variable #6999 to access the parameter value.