I use the Haas built in text marking function on my VF3 mill. (G47)

It works nice in most cases, but when I use certain numbers next to each other (like a 0,8,6,9), they are crowded together to the point it looks bad.

G0X0Y0
G47 E10. F5. I0 J.05 P1 R0.1 Z-0.005 (0869)

Is there any parameter that will space these characters out?

Bill



(E VERTICAL FEED)
(F CUTTING FEEDRATE)
(I ROTATION)
(J LETTER HEIGHT)
(P SERIAL 1 LITERAL 0)
(R RETURN HEIGHT)
(Z CUT DEPTH)
(TEXT)

Bill,

You might try a space between the numbers..say 0 8 6 9.

It could just be that at .050 high lettering and a cut depth of .005 they just run together.

So you could try a slightly bigger letter height and the same depth of cut or same height and a smaller depth of cut.

Also the size of the ball mill or the size of flat on the end of your engraving tool could be contributing to the problem.

By that I mean if you where to use a 1/2" ball end mill at those setting you would just get a mess of lines instead of clean lettering.

I ran a test piece with different depths on my 0.050 height letters. (I have to use 0.050 high). My tool is a sharp point 45°. All the numbers look good except the 9 overlaps onto the character before it. I think a space would be too big of a gap.
I will probably just add another line and put the 9 where I want it.
You can see the deeper I go the more the overlap.

I was hoping there might be a way to modify the built in code.

I wrote to Haas (answerman@haascnc.com) about this and got an answer today. The text is controled by program O9876. You can edit this at your own risk so make a backup copy first.

He sent me a copy of the program if anyone needs it.

It looks like it uses incremental programming and is based on 1" high characters. To add extra space I just need to move the position of the starting point for that letter.

I have not tried it yet but it looks straight forword enough.

Bill

Well, I'm stuck again. Program O9876 is not avaliable on the Haas control to edit. I know it is there because I can see it execute in single step with setting 74 on (9xxx PROG TRACE).

I have setting 23 (9xxx PROGS EDIT LOCK) off and can see O9999 (quickcode) and O9000 (pallet macro), but cannot see O9876.

I am thinking that if I load the O9876 into the cnc from a floppy, it might override the built-in program (that I cannot see) and allow me to edit.

Does anyone know if this is correct? (the Haas guy is out until Oct.1)
Bill

Problem solved. The built in version of the O9876 text program must have been an old revision. The new one fixed the problem without having to edit. When you load in the new program it overrides the built in program. Its nice to know I can edit the letters if necessary.
Bill