Question about length offsets ?

[hall6ppc]

Hello , I have a 2004 HAAS VF1 .My question is when using G54 work off , I have noticed if there is a value entered into there length offset section (Z) of G54 it will add this value to my tool length off set when I set up a new tool . However it will not do it with any other offsets G55, G56 etc. Why is this ?

Thanks for any help !

[Geof]

Originally Posted by hall6ppc ...... Why is this ? Thanks for any help !

Probably because you have Setting 64 turned ON. Here is a description copied from the Haas manual.

64 T. OFS Meas Uses Work

This setting changes the way the Tool Ofset Mesur (Tool Offset Measure) button works. When this is ON, the entered tool offset will be the measured tool offset plus the work coordinate offset (Z-axis). When it is OFF, the tool offset equals the Z machine position.

(I think) it only works with G54 which is the default work zero.

[hall6ppc]

Originally Posted by Geof Probably because you have Setting 64 turned ON. Here is a description copied from the Haas manual. 64 T. OFS Meas Uses Work This setting changes the way the Tool Ofset Mesur (Tool Offset Measure) button works. When this is ON, the entered tool offset will be the measured tool offset plus the work coordinate offset (Z-axis). When it is OFF, the tool offset equals the Z machine position. (I think) it only works with G54 which is the default work zero.

thanks I will change it to see if does anything .

[laurencen]

this z setting in g54 is great if you set all the tooling to a standard bar such as 10 inches long, all tools are set to this, now when you are setting the work on the table all you have to measure is the distance from the bar to the work and all tooling is correct to the work, if you change the block on the table enter the difference and again all tools are set, I have not tried this woth g55, matbe it has to be turned on in parameters but thos z input is sure a handy feature

[Pondo]

Originally Posted by laurencen this z setting in g54 is great if you set all the tooling to a standard bar such as 10 inches long, all tools are set to this, now when you are setting the work on the table all you have to measure is the distance from the bar to the work and all tooling is correct to the work, if you change the block on the table enter the difference and again all tools are set, I have not tried this woth g55, matbe it has to be turned on in parameters but thos z input is sure a handy feature

If you are touching off tools to a common Z point and then G54 Z0 = the distance from there, then you want setting 64 OFF unless you are touching off tools to the actual workpiece Z0 for some reason.
For example, I touch off the tools to the hard jaw of the vice. The G54 (or G55, G56, etc.) Z offset is the distance from there. Whenever I put in another tool I touch it off to the vice. If I have to add a tool and can't reach the vice because of an overhanging part, then I touch it off to that part's Z0 surface and then add the inverse of the G54 Z offset. If G54 Z0=2.005, then I subtract 2.005 from the offset. That is what setting 64 does. If I had setting 64 ON and touched a tool off to my vice, it would crash pretty hard when I ran it.