Can someone explain how to use this

What I can do at this time my post processor outputs the g41 with a p3  this results in the dia. Offset to be set as indicted on the screen

Eg tool = 6
Dia. Offset =6
H offset =6

Now which way do I set the value in the tool table ?

I need this as I am making a bearing with a grove on each side ( made with a woodruff cutter ) and it needs to fit hence the need to set CC I am talking about 0.02 mm

Thanks in advance

Stuart

Stuart, What are you looking for?
You don't set the direction G41/G42 in the tool table, you only set the diameter in the tool table.  
I have only used cutter comp a couple of times and haven't used it since I started using Fusion 360. So I'm not the best to explain how it works, but here are a couple of resources that are informative.

Have you read through the cutter compensation section in the mill manual?  
Page 52
http://www.machsupport.com/wp-content/uploads/2014/05/Mach4%20Mill%20GCode%20Manual.pdf

John Saunders has a pretty good video on his YouTube Channel NYC CNC.
https://www.youtube.com/watch?v=Mxtfs0Wr2X0

Thanks Chad

Yes I am ok with the g41/g42 is from the cam and is outputed by the post processor
Sorry I I did not make it clear with the tool table the tool is set by the dia. Column and the dia offset in the dia. Offset. Column

Yes I do use fusion360 for cad/cam

It was when using g41 do I input a - value in the offset table or a + one

These parts are for a beam engine and are tiny about a 10mm cube when made they are split to form bearing brasses

Thanks for the links I will give them a good looking at more than once at 71 the remaining brain cell is slow

Stuart

I'm not sure,  it will change depending on where you are cutting, inside or outside profile.

I would just do a quick bench test and see what is going to happen.  Put a (-) value in and see where it is going to cut.  If that is wrong, put a (+) value in. 

funny you should say that , I have just cad/cam up a simple part to do just that.


got some parts in the mill at the moment for the watts parallel motion to make as there are a few its set up to do multiple parts

I will come back with my finding. and broken end mills


Stuart

Thanks for your time

Well it worked out ok

Minus value did make the bored hole bigger


Stuart

It looks like you solved your problem.  However, in the event this helps clear things up further, most commercial cnc machines, machine controllers, and cad/cam software packages use cutter comp the same way.  A negative cutter comp value would signify that the tool is smaller than programmed for, and will move the center of the cutter closer to the edge being cut, which will result in removing more material from both inner and outer contours, making inside holes and pockets (i.d.) bigger, and out side dimensions (o.d) smaller.  The opposite is true.  A positive cutter comp value signifies that the tool is larger than programmed for, and will result in the tool being moved farther away from the programmed edge and leave more material on the part.  typically, the cutter comp value entered is treated like a diametric value, and will result in the tool being move half that distance away from the programmed path.  For example, a -.010" cutter comp value with result in the tool (let's say a .250"Ø end mill) being treated as though it is really a .240"Ø end mill, and this will result in the tool path being adjusted so the tool is moved .005" closer to the programmed part edge, effectively removing .005" more material that it would have otherwise.  in and hole being milled in to a part, .005" of extra material would be around the entire perimeter of the hole resulting in the i.d. of the hole to be .010" larger.