getting program zero on Okuma LB12

[roger_e]

Okay,

we can get programs from our PC to the OSP500l-G no problem now.

we will use visual lathe to program (right now I am writing the code in notepad) so we can avoid using the OSP to program....but how do you set part/program zero.

My experience: touch part off and cut just a little bit(face part off), set z to 0. then load program. cycle start. make money

How do you tell the Okuma Lb12 using OSP 500l-g where part zero is?

[underthetire]

Same way. Find your master tool, like tool 1. Set the tool offset to zero on Z for that tool. Touch face of part, then go to zero set (softkey at the top of the keypad). cursor to z and press cal 0 at the bottom of the screen. All other tools are then set normally for Z axis. The rest of the tools are then set from tool 1, so the offset should reflect the length of the tool in relation to tool 1. The X axis is all based off a centerline between a boring bar holder and the spindle. So drills would have a 0 value for x axis on the tool offset page. If this is not the way your machine is, you can sweep in a boring bar holder with a co-ax indicator, then use the zero set again, but this time go to X and calculate 0. Keep in mind that Okuma uses a absolute encoder, with a actual value from 0 to 999.999 inches, so machine position will be strange number that makes no sense to you. If you see a 406.992 number or whatever, thats just where the encoder is at when it was put on. Does not affect operation at all, and is totally normal on an Okuma.

[Algirdas]

You can memorize offsets in program also.
VZOFZ=44212.21
this is Your readings of Z axis zero after OSP calculated it on zero offsets screen.
VZSHZ is zero shift of Z axis.
and so on