Re: BobCAD/CAM v.s. Dolphin CAD/CAM

Chris,

Using the cutter comp routines on Dolphin is a doddle (when you know
how!).
Like John S., I only use them when working to tighter tolerances, but
it would apply equally if you are unsure if the cutter you will be
using is a re-grind or not.

If I was using Dolphin to machine an irregualr shaped pocket, using
one tool, I would approach it thus (CAM):-

1/Define your tool, you will have to give the CAM system a 'nominal'
tool diameter so that it can work out its area clear toolpath, it
doesn't matter if the tool is 0.01" - 0.02" under size.
2/Select your tool, not forgetting 'cut depth' to create the roughing
passes in Z
3/Select area clear, define the type of routine you want to apply,
and leave say 0.02" for XY finish.
4/Select go-round, leave XY finish at 0, select tool offset
(LEFT/RIGHT), select your required approach & departure, on the
options tab select 'Ignore CutDepth settings for tool' (ensures
single Z depth pass).
5/Check on the graphics that the tool offset is correct, double click
the last go-round on the operations menu, and on the options tab,
select use 'part surface', when you post this it will output the
finish component sizes (not offset toolpath) and G41/G42 or whatever
your controls comp commands are, for the last go-round only.

I would use the arc approach/departure options with use part surface,
note that it actually does a 'teardrop' move, a linear move into an
arc, this ensures that comp is applied on a linear move which is
required by some CNC controls. You could also select a normal
approach which is a perpendicular approach to the geometry designed
for applying comp.
As Mike Milligan stated in an earlier posting, the comp routines are
affected by the post processor being used, so this method may not
work with every post processor, it depends on what the original
customers requirements from the post processor were.

If anyone would like an example of this, contact me off list and I
would be happy to e-mail one out.

HTH

Dave Pearson