Newbie- best (easiest way to increment Z depth)

[Castle1]

We don't have the Macro option, although I enabled the timed demo mode so I could use variables. Would anyone know of a simple way other than copying and pasting & making the program longer than it should, a way to increment the Z depth per pass, I was thinking there should be a G91 way of cutting an arc with cutter comp, then moving back to the beginning and lowering Z another .050, for a total of -.650 Z depth. Code is below,
Does anyone know how much the Macro option costs on a TM-1 2007 model?
Without variables because we wont have this after the demo runs out.

Thanks for any help.

O00011 
#100= -.050 (VARIABLE 100 SETS 1ST Z DEPTH) 
N10 (T5 .501 4FL EM) 
T5 M06 
G54 G90 G00 X0.5 Y-1.8 
G43 Z0.5 H05 
S304 M03 

N150 G00 X0.5 Y-1.8 
G01 Z#100 F20 
G01 G41 X0.3 Y-1.7022 D05 F10. (D5 IS NEEDED)
G02 X-0.75 Y-2. R2. F1.8 
G01 X-1.01 
G01 Y-2.3 F20 
Z0.5 F20. 
G40 
G01 Y-2.5 F20 
#100= [ #100 - 0.050 ] (DECREMENT Z AMOUNT)
IF [ #100 LT -0.65 ] GOTO200 
GOTO150 
N200 G40 
G01 Z0.5 F20. 
G00 Z7. 
X2. Y1. 
G53 G49 M05 
M09 
M30

[Geof]

You can do it with nested subroutines using an L count with the M97.

What is it you want to make, hole, pocket, step down a perimeter, ??

For interpolating a hole of course you can just use G91 and L right in the interpolation command;

G91 G03 I J Z-.1 L10

will do ten counterclockwise interpolations moving down -0.1 every time for a total of 1.0.

If you can give me some sizes I might be able to give you some sample code the way I would do it.

[Castle1]

It is a steel rectangular bar sticking out of a vise, with a 2.0" clockwise arc.

see attached

Then I will rotate 90 and put the same doubled (mirror image of the same)

[Geof]

Is that a top view? You want to take the arc in several cuts rather than one cut?

[Castle1]

Yes several cuts , then a finish cut.

[laszlozoltan]

Sorry, but I have to say I was looking at a HAAS awhile ago, but I didn't know this that they would choose to reward their customers choice by charging them extra to enable such a measly little macro that would make their mill a bit more versatile. Booo on HAAS man, Boooo.

[MILLMARK]

You can turn the timed demo off after the program is written/loaded, and the machine will still run it. If you remember to turn it off every time, it'll last a long, long time.

[Geof]

Here it is using a 3/4" mill (enter 0.75 in the tool diameter on the offsets page.)

I am using 1" square material

The work zero is placed at the corner of the material.

T1 M06 (3/4" MILL)
etc
etc
N1 G00 X0.4 Y0.4 Z0.0
N2 G91 G01 Z-0.1 F50. M97 P100 L10
N3 G90 G01 Z-1.05 F50. M97 P100 L2
N4 G90 G00 Z1.0
etc
etc
etc
G53 G00 Z0.0
M30
-------
N100 G90 G41 D01 G01 X0.0 Y0.0
N101 G02 R2.0 X-1.732 Y-1.0 F20.
N102 G40 G00 X-2.0 Y-1.4
N103 X0.4
N104 Y0.4
N105 M99

Line N1 moves to the start point.
N2 increments down Z-0.1 then goes to line N100
N100 moves to the corner and sets tool compensation, notice we are back in absolute (G90)
N101 does the radius
N102 cancels tool compensation and moves away
N103 moves to the X coordinate for the start point
N104 moves to the Y coordinate for the start
N105 returns to N2
N2 increments Z down again and goes to N100
When L has counted to zero N105 returns to N3
N3 moves the cutter just below the bottom of the part and goes to N100 twice for two finish passes
N4 moves Z clear


I think I have got it correct but I haven't checked this on a machine. You can run it in Graphics or do a dry run without any tools or material.


Laslo; There is another way to look at the way Haas prices their machines. If I don't want Macros, which I don't because I can't be bothered learning how to write them, I can save a couple of thousand dollars on the machine price and spend it on tooling. I have found because Haas has local subroutines that are tacked on the the end of the main program, can do subroutine calls with an L count and can nest subroutines many times deep I can do a lot of things that would need macros on a different machine.

[Castle1]

Thanks Geof I'll try that out when I get back to work . I'm taking a week off so it will be awhile until I can try it.

Thanks for the tip MillMark, now are you saying that the Macro option can be off and it will still run? If so I can program off line with variables and it will load in and run too? With macro demo off that is.

Thanks again everyone!

[MILLMARK]

The demo must be on to load a program with macros, or to write any macros at the control, but once the program is in the machine you can turn the demo off, and the program will run. I realized this while using G47 text engraving, which is all macros, on a mill without the macro option