Re: What does Tool Radius Compensation do ?

Jon Elson <jmelson@...> wrote:
Subject: Re: What does Tool Radius Compensation do ?

hansw wrote:

> My MAXNC software claims to have
>
> "TOOL RADIUS COMPENSATION "G" codes (G40, G41, G42)"
>
> and the Program by Doug Yeager "CNCPRO.EXE" does not have this. I
> prefer the Yeager program, it's much more logical in it's user
> interface.
>
> What is "TOOL RADIUS COMPENSATION " how can I see the difference
> between the results of with and without it...

Your program (toolpath) must activate it, and you must have already entered
a radius (or diameter, usually) for a specific tool into the CNC's tool table.
It allows tools of somewhat different diameter to be used without changing the
program. The CNC has to know which side of the specified line to cut on.
The toolpath is specified as the actual dimension of the part, and is not
offset
by the tool radius, as you would usually do when writing G-code by hand
or with a CAD/CAM program. Then, when the program is run, the CNC
control uses the tool's radius to offset its movements to one side or the
other from the specified coordinates. See my desciption of this at
http://206.19.206.56/diacomp.htm Also, you might find a lot of interesting
info in the CAD_CAM faq, at http://206.19.206.56/cadfaq.htm

[While there was a lot of interesting information there- thanks for your
efforts on this, Jon- I was disappointed to find that about half the links
didn't work. Specifically, I got a "404 not found" error for the pages with
URLs ending with: preset.htm, stepper.htm, Bobcad.htm, cmm.htm, dnc.htm,
ecm.hcm.vmc.htm, hmc.htm, tc.htm, vbm.htm, hbm.htm, quill.htm, vsd.htm, and
srvodynm.htm. And stg.htm gave a javascript error. ]

> The kind of things I do, I have not seen any difference... Dumb Fat and
> Happy... but would like to understand this, what am I missing...

The big advantage here is that you can use re-sharpened cutters, which are
usually a little under-size, if the side cutting flutes have been re-ground.

A cute trick I use is to run the program several times, first with the cutter
diameter entered into the tool table larger than the real size, and then
reducing
the entry in the tool table. This allows one program to be used to make
roughing passes, and then a final cut. As the offset is made smaller, the
tool will cut closer to the line specified in the toolpath program.

Jon

[Actually, the reason I was searching in there was related- or might be
related- to this tool-offset issue. I've been trying to make 360 degree 3d
parts using a mill equipped with a rotary table, taking instances of a part
and milling one "view" up to about half-way down, then indexing over 120
degrees and milling another "view", etc. Since I'm zeroing the y and z axes
to the axis of rotation, and am rotating the part representation along an
axis established in the CAD geometry, it seems to me that everything should
line up nicely, but instead I'm finding that the instances are offset from
each other by a discontinuity that seems suspiciously like the radius of
the 2mm cutting tool I'm using. Am I zeroing it wrong, by making the Y
zero-point the middle of the tool and not one edge or another? Am I off in
the Z-axis by zeroing to the tip of the ball-end tool and not the point
where the ball diameter falls? Should I be invoking tool-offset
compensation? (This would be bad, if so, because the MaxNC software I'm
using gives a choice of this or unlimited file-sizes, which I need.) I
haven't reground the tools, so I thought DeskProto should be giving the
correct commands. I'm using a "spiral out from the center" milling
strategy, where the tool cuts on each side of the part alternately. Is it
assuming that I've got a mill that automatically compensates for tool
offset? Any ideas out there?]

Andrew Werby

Andrew Werby - United Artworks
Sculpture, Jewelry, and Other Art Stuff
http://unitedartworks.com