When you say this has been written with no tools - I take it you mean drawing tools etc.

Before I could suggest an answer ( and I am not the best man to ask, but it is an interesting question) does your G Code include any Tool information - is your tool table up to date etc. I seem to think it must be because you are asking about tool wear.

Have you already used tool width offsets etc in the code, or have you written the code allowing for this in the writing.

If you have written with tool width offsets already in, then just decrease the tool dia by 20 thou and run exactly the same program again. This would, in effect be the same as adding 20 thou wear to the tool - although I have never used tool wear - and you have the added advantage of knowing the original program worked.

I think I understand your question, so I will ramble on a bit. Pick out the bits you need.

In simple milling, you are normally cutting a shape out of a flat material. This  involves using and end mill, or a slot drill or some similar tools.
Since they all go in the same  chuck, then the path they cut depends on their diameter.

G Code allows you to program the cutter as though it had no diameter, and so what you see on the Mach3 tool screen is the actual program you write.

Tools you use in the mill are entered into the tool table - see Config/Tool Table - and in there, for each tool, you can enter their diameters, lengths etc etc. Wear, which you keep mentioning is also included, but I do not use it, because I measure my tools with calipers, and enter that diameter in the table. I assume the big boys buying super duper tools will have a specified diameter - and add wear in microns or thous as it happens to maintain absolute accuracy.

Tools are changed by codes M6 T** the numbers following the T is the tool number in the table. The M6 code can be programmed to do several things - nothing, move to a specific location for a manual change, or operate an automatic tool changer.

Cutting a simple outline - and allowing for the tool diameter is G41 or G42 - G41 is with the tool on the left, G42 is with the tool on the right - G40 cancels the compensation.

All you do is, at the begining of the program enter G41 - and from there until a G40 cancellation, the machine will alow for the tool width of the tool that is currently being used. It changes the compensation if a new tool is added.

I do not understand, when you say you want to use "wear" to change the part dimensionally when you cut it - how many go's are you having. In theory if your machine is set up accurately, and you draw you part accurately, then the machine will cut it accurately, without, as we used to do manually - working up to the finished diameter in little cuts.

Machines can be programmed to take roughing cuts and then change tools and take a fine finish at exactly the right diameter or whatever.

Have a look through the codes on Mach3 Mill and you will see what I mean. Have a look through Mach3 Config as well.

Thanks It's starting to make sense.
When I say wear, what I think I should be able to do is; if I need to cut
.002 more off a side I "in theory" should be able to go into "tool wear" and
put in -.004 and that should cut .002 more off the part.
? How would a simple code look like if I wanted to use a 3/8" endmill 1" long to cut a "2 inch circular pocket"  .500" deep
(so I guess the cutter would be on the right if I was cutting cw)
I need to know this so if I want to change to a .5625 cutter I won't have to redo the whole program.
Please let me know,
Thanks,
Brian

Basic circle code is this :-

G00 X0 Y0 Z1.       (move to centre of circle)
Z.05               
G01 Z-.5 F2.          (feed into job)
G41 P.375 X1. F4.  (comp on P=cutter dia X= radius of hole)
G03 I-1.                (cut full circle)
G00 G40 X0           (take comp off)
Z1.                       (rapid clear)
M30

Graham.

Thanks Graham
I think with all of your help I getting it to work.

Thanks again

P.S.  What's the best book or cd to learn G Code
        I'm not an idiot but I have been called a monkey before
        Monkey proof is best.

Just search the web, there are lots of g-code sites.

By the way, you can not be an idiot if you chose Mach3. 

Graham.

I keep getting a fault " tool radius is greater than approach line 7"
What does this mean?

Is the I figure in the G03 line the same as the X figure in the G41 line ?  If not it should be, but minus.

G41 P.375 X1. f4.
G03 I-1.

It also uses inc IJ mode.

Graham.