Re: Measuring accuracy

--- In CAD_CAM_EDM_DRO@yahoogroups.com, Gregory Kamysz
<smsupply@a...> wrote:

> All
> of the demos use relatively coarse settings, obviously to shorten

CPU

> time, and they don't tell you what realistic settings for accuracy

are.

The settings in DeskCNC calculate scallop height. If you have a .0000
scallop height one would expect the user to be savvy enough to
realize that this is not realistic. The toolpaths also are displayed
graphically and in dynamic 3D. If there are cuts everywhere that are
not where you would want, it is expected that you have enough problem
solving skills to experiment with your settings and to develop a more
efficient cutting strategy. The design philosophy for StlWork was
that it is a tool for people that need a sophisticated 3D cam
machining program on a low budget. It solves that design intent very
well. It is not designed to be a trainer or a toy.

> The software seemed intuitive to me but in fact, it's not. Now,

I see

> where the issues are with time and finish. All of my problems

relate to

> these settings.

That's correct. StlWork has the simplist interface we could develop
while still packing in some extremely powerful capabilities.

> > Right tool #1...............
> > Right Tool #2...............
> > Right Tool #3...............
>
> Here is my plan, tell me if I'm wrong. Increase the resolution of

the

> STL file.

Don't increase it beyond 1.5 times the surface accuracy you plan to
machine, it will just make the file needlessly larger, and the
display and computation time will rise geometrically.

>The square stock is to hold the part so that the top and
> bottom can be cut in two operations.

I would go with roundstock and machine the leading and trailing edges
through the hub on a CNC lathe. Leave a locating and stabilizing ring
around the OD. A CNC lathe is much more efficient at removing large
volumes of material than a mill.

>Make a model without pockets(the
> center recesses) to skip these steps which the software can't

handle

> well.

Model just one blade (then use a rotary table to index to each blade
of your part) and one toolpath, or just the three blades and 3D
surface mill just those, stopping short of the surfaces of the hub.
Draw just what you want to cut. With StlWork you can restrict the
cutting zones to this area and are not required to cut the entire
model,
and with the no-flats you can actually machine just one
blade out of an entire model. It will even let you create multiple
zone selections (one for each blade) as cutting strategies and will
produce a single program consisting of the 3 vane selection area
programs. You could probably use the water line to cut the hub too,
but a simple multiple pass to depth contour from a drawn circle is
hard to beat for generating G02 code for this part.

>Write the code to cut these areas. I could care less if the area
> between the blades is accurate or not as it will all end up as

chips.

That's right. This is the area that I refer to as the pocketable
portion. You can look through the part in these areas. Use the
largest cutter possible and have at it.

> I guess I don't have much of a choice without putting in quite a

bit of

> effort to use a G02 to finish the outside of the round hub portion

of

> the part. One option would be to make this oversize in the model

to

> allow for separate hand coded finishing. With what I know now it

may

> not be necessary.

Like I said, this area is a good job for a CNC lathe, or any 2 1/2
axis cad-cam if you do mill it.

> Where does one purchase bull nose endmills in small

sizes, .25", .125"?

mscdirect.com has between 500-600 different sizes in stock, all
cobalt or carbide, and including 1/8 and 1/4. J&L also carries them.

Search for endmills, then radiused corner.

Here is a sample part number too: 00427278

Fred Smith - IMService