How to Input New Tool?

[ggundrum]

Hi All,

I have a Bridgeport XV1000 with a 24 tool changer and a Fanuc Oi-mc controller. There are over 100 programmable tool offsets on the controller and I want to start utilizing more than 24 tools.

My question is: If Tool 1 is in Pocket 1 of the tool changer carousel, and I replace Tool 1 with Tool 50, how do I tell the machine that Tool 50 is now in the tool changer carousel position that Tool 1 used to be in?

Is there a way to view what Tool is in what position in the tool changer carousel? I know that in MDI, you can see the tool in the spindle and the tool in the tool changer that is in position to load, but how do you view the position of the other tools?

Hopefiully there is a simple solution to this, thanks!!

[angelw]

Originally Posted by ggundrum Hi All, I have a Bridgeport XV1000 with a 24 tool changer and a Fanuc Oi-mc controller. There are over 100 programmable tool offsets on the controller and I want to start utilizing more than 24 tools. My question is: If Tool 1 is in Pocket 1 of the tool changer carousel, and I replace Tool 1 with Tool 50, how do I tell the machine that Tool 50 is now in the tool changer carousel position that Tool 1 used to be in? Is there a way to view what Tool is in what position in the tool changer carousel? I know that in MDI, you can see the tool in the spindle and the tool in the tool changer that is in position to load, but how do you view the position of the other tools? Hopefiully there is a simple solution to this, thanks!!

When you replace an existing Tool Num 1 with another tool, the new tool is also referenced as Tool Num 1; you can't call, for example, T50 in your program.

Depending on the Offset Option your control is equipped with, you may have separate offsets for Tool Length and Tool Radius Compensation, or both types of offsets may have to be accommodated by the one offset registry. If your control is the latter, then you could use offsets 1 to 24 for tool length and 31 to 54 for Tool Radius Comp. Many programmers use a system of adding a constant to the offset numbers used for Tool Length to specify the Offset Num for Tool Radius Comp, and in doing so, some numerical relationship is retained with the Tool Number. In the example 31 to 54, the constant used is 30. This is more logical than using Offset Num 1 for Tool 1 Length Offset and, say, Offset Num 99 for the Radius Comp for the same tool. Offset 99 has no numerical relationship with Tool Num 1.

If you wanted to have the tool length offsets for a number of tools in-excess of the tool magazine capacity preset and ready to use in the control, you could use a similar system by adding a constant, say 50, to the original set of tools. For example, T01(1) would use Tool Length Offset H01, and T01(2) would use Tool Length Offset H51. Calling the tool and offset for the two different tools that will be specified as T01 would be as follows:

(FIRST 24 TOOLS)
T01 M06
G90 G54 X0.0 Y0.0
G43 Z10.000 H01

(SECOND 24 TOOLS)
T01 M06
G90 G54 X0.0 Y0.0
G43 Z10.000 H51

This practice would require impeccable record keeping and checks to ensure that the correct tool for the corresponding Tool Length Offset was being used. The time saved by having the tool lengths pre-registered in the control could be wiped out many times over by one prang caused by the incorrect offset being applied.

Regards,

Bill

[underthetire]

Check on your tool registry page. Most random side mount atcs will let you. For instance, I'll call my probe tool 99, but it's in pocket 30. Some machines can, some can't. It's not up to the control, it's how the MTB implements it.