Re: [CAD_CAM_EDM_DRO] Visual Mill vs Visual Mill Basic questions

Michael,

> I'm looking at all these things that the full package does, like
> "horizontal re-roughing" and I'm finding that a lot of them don't tell
> me much, coming from a "try to remove only the metal I don't want,

In general, z-level (also called horizontal) roughing is the best routine
for roughing shapes, because it combines the strengths of normal endmills
with the more robust axes of a most machine tools - X & Y.

The toolpaths are generated by stepping through the height of the model in
'layers'. Generally shallow depth cuts at higher speed gives good results in
metals. Larger endmills are used for the first pass, then a 're-roughing'
routine is run with a smaller diameter cutter to remove material left by the
larger cutter. (inside corners, inside fillets, etc.)

In the re-roughing case, the program is 'aware' of remaining stock. The
re-roughing routine saves much time that would have been spent by the
machine 'cutting air' - re-cutting most of the previously cut areas.
(VisualMill happens to allow using several different types of cutter to
rough with, and then different types to re-rough with if you'd like.)

Parallel or 'raster' cuts were first to arrive on the 3D scene a number of
years ago. It involves taking a slice of the model in the vertical plane,
and offsetting the center of the cutter (original method) or the tip (more
recent) to get a path for the tool tip. This is done across the model, with
the resulting toolpath looking somewhat like a venetian blind laid across
your part. It used to require a ballnose cutter - simpler math. Not all
programs would let you 'climb' cut exclusively, either. (Climb cut only, in
parallel/raster, is sometimes called a 'box' cycle. This is because the
cutter path lifting and traversing back to the next cut line makes a 'box'
shape.) This was important when roughing a shape in steel. Now that z-level
routines are around, it isn't as important.

Roughing areas with a ballnose is MUCH slower, because you are limited by
the cutting speed near and at the tip of the radius, and the need to limit
the 'scallop' height of material left between the cutter paths.

Parallel paths with ball or bullnose cutters ARE a standard (and good) way
to finish machine the last 0.010" to 0.015" of stock, left by the roughing
passes. The roughing is calculated to leave manageable 'steps' in the
roughed out material.

> I suspect that many of those features may be things that allow the
> job to be done faster, or are "conversational programming" features
> that let you avoid doing a 3D drawing/G code program to make
> things.

Visual Mill is not what I would call 'conversational programming'. The
features give higher levels of control over the toolpaths. To me,
re-roughing isn't as important as pencil tracing/valley re-machining,
constraints to machining within certain angles (hill/plateau), and the
graphical toolpath editor.

> Do any of those things actually let you make something
> that you couldn't make with the Basic version.or that a skilled
> master machinist (not me) could make on a manual machine?

Not necessarily make something different, but potentially quite a bit
faster, and with better surface finish control. Manual isn't a comparison
with free form 3D shapes, they are out of the range of a manual machine, no
matter how experienced the operator.

> I suspect that I'm not the only newbie who wonders what all this
> stuff is, and why it makes a difference, and would appreciate any
> light that the experienced members of the group might be willing to
> shed on the subject.

What it is is because of the difference it makes, which is more fully
realized after getting your feet wet and doing it. Start with cheap/free
programs, and after a year or two, look at what you can do versus what you
need to do.

> It seems like the Basic package would let me
> do everything I could do on a manual mill, as well as stuff like
> smooth curves and transitions that are often a "get it close on the
> mill and then get out the big bastard file" now.

VisualMill Basic sounds like it might work for you, but may not have the
drawing features you'd want. Some others you might try looking at are
Dolphin Partmaster, Vector, Rhino (CAD program only), IntelliCAD (CAD only,
was free), SprutCAM , OneCNC 2003 products (XP is another cost/performance
level).

Be aware that drawing program and g-code generation do not have to be the
same program.

Hope this helps,

Keith

(No ties to VisualMill, other than pleased commercial user of VM5.0 full
version)