[LYN BYRD]

Anyone have a list of Dos commands that can be executed from the program.
DPRINT, SET, CLR .....etc?

[tskguy]

Google machine to the rescue,

MS-DOS help and commands

Im assuming you are using MS dos or a Command prompt in XP.

E

[LYN BYRD]

They might be specific to Milltronics machines.

[ZZZZ]

These aren't DOS commands, they are part of the Centurion control. Look at the Parametric Programming section of the programming manual, they are described there.

[ZZZZ]

The ability to use parametric programs (or parametric lines in a conversational program) combined with the 'open architecture' of the control means you can have a program do just about anything you can think of.

I have written code to check for broken tools using a simple switch, check for pressure on a hydraulic clamping fixture, check for vacuum on a vacuum table, stop a program to ask for input, use the handwheel to re-set an offset in the middle of a program, and lots and lots other things.

If there is something you want to do, post it and I'll try to help.

[LYN BYRD]

I am setting up offline tool measurement (H & D offsets).
I do this now (presetting tools), but I have to manually input the data to the control. I have 5 Milltronics machines. It would be nice to have the gage send the data to a shop pc and the control read the data from there.

[ZZZZ]

I think you can do that by organizing your data for each machine into a file that you can Verify or Run at each machine.

The offsets are stored as parameters and you simply need to load the new offsets into the parameter file.

Older software versions used P501 - P599 for the radius offsets and P601 - P699 for the height offsets. P501 is the radius offset for tool #1, P650 is the height offset for tool #50, etc.

Newer software uses P2001 - P2099 for the radius offsets and P2101 - P2199 for the height offsets.

You can find out which ranges each machine uses by going to MDI and typing P1=P1501 then go to Parms - User to check . If P1=0, you have an older version, if P1 does not equal zero, you have a newer version.

The data file should look like:

G10 (allows writing to the Parameters)
P501=XXXX
P502=XXXX
.
.
.
P601=XXX
P602=XXX
G11 (closes the Parameters)

Of course, use the appropriate P numbers for each machine.

Good luck, let us know how it turns out for you.

[LYN BYRD]

So, I would create a program that would contain the h & d offsets (using the correct P number) and read it into the control and run it?

[ZZZZ]

Exactly right. When you Run or Verify the "program"you created from the tool setter, you load the values into the tool offsets table.

Be aware that the values you get form the pre-setter are usually from the gage line on the toolholder to the tool tip, which is different than the distance from Z home to the top of your part that you get with the Z-Tool or TLSet techniques. You will need to use the Work Coordinate Z offset to get the tool to the right place. You can NOT mix the pre-setter values with the Z-Tool values without causing yourself problems.

Use one or the other, not both.

[LYN BYRD]

Normally, I have actual tool lengths in the offset page and just set the Z coordinate for part zero.
Thanks

[ZZZZ]

Good, this should work fine for you.

I won't normally recommend this technique to less sophisticated users, but you don't fit that description.

[LYN BYRD]

I quit touching off tools on the machine about three years ago and have not looked back. It was amazing on how much time it saved me by presetting tools.
I don't know why anybody would want to touch off every tool on every part on every job. Thanks for your help

[ZZZZ]

You're welcome, glad I can help.