Face mill macro?

[mmachining]

First off I have a vf-2 and 3 ,was wondering how to check if I can run macros on them? Secondly does anyone know where I could get a macro help or a macro program that allows me to enter in the thickness the size x and y of stock and it goes from there. I use the same face mill for everything so that won't matter and I use the same G54 for everything as well. Any help would be great. The machines are mid 90's.

[Mic6]

to check if you have macros installed: in MDI "#1=100" cycle start. If it alarms, no macros. If it takes it, start writing.

[kendo]

ok, heres mine
Be ye warned however, this is my first real macro
I tested it out on a couple different blocks and it worked as expected, but whatever problems I haven't foreseen will be yours to discover. As with any program handed to you, you should run this at 5% rapid with your hand on the red button the first few times. And give yourself a Z-offset and cut air at first like I do.

This macro faces a a block in a bi-directional manner, climbing one way, and conventional the other way. You must start with the cutter at the center of the block, and your work coordinate X0 Y0 must be the center of the block. It will rapid to the back left corner and rapid down in Z then at the end of each cut it will rapid in Y to the next cut. It will start and end each cut with .25" clearance between the edge of the block and the cutter so there shouldn't be any problem with the rapids as long as your inputs are correct. The cutter will come up to a clearance height of 1" and rapid to the back left corner again to start over when making multiple depth cuts. When the operation is comlplete, it will rapid back to the center of the block.
Heres an example of the macro call:

G65 P9010 X12 Y12 Z-.5 D2 W.75 Q.125 F100.

W = cut width expressed as a percentage of the cutter diameter in decimal form
X = size of block in X
Y = size of block in Y
Z = total depth, this must be a negative number, if not, it will be changed to a negative number
Q = max depth increment, this may be omitted if you only want to make one pass the Q value doesn't have to divide evenly into the total depth, but if it doesn't, the number of depth cuts needed will be figured and the total depth will be divided by that to calculate the actual depth per pass
D = diameter of the cutter
F = feedrate, this value must include the decimal

I've aliased this macro to G26 in my control by setting parameter 91 to 26
so I can call it like this:

G26 X12 Y12 Z-.5 D2 W.75 Q.125 F100.

One more thing, I found that if the cut width divides evenly into the size of block in Y, then the last cut will be right to the front edge of the block.
The macro checks for this, and adjusts the initial starting point and adds an extra cut in order to avoid that scenario.

I don't know what the differences will be from my control to yours so beware.
I think theres enough notation in the program for you to figure out whats going on, and hopefully you can study it and figure out any needed changes.
Maybe it'll even help you learn to write your own macros.