Ken, There are several issues going on with the parts you are
receiving, and I will at this point eliminate the machine as the
issue, because from what you are describing, there are other
fundamental issues at work.
I have a question for those doing CADCAM wax master patterns,
How much finishing do the patterns you send to your customers
require, Reason I'm asking is I have been getting masters that
still are showing tool marks on the back, some still have a
significant degree of flash in inside cuts, and nearly all look as
though the outside edges were filed with a checkering file!.
The flash on the inside cuts are due to the fact that the machinist,
finished the through cut precisely to the required depth, and when
the item was flipped and the rest material was removed to bring the
material to thickness, they were both pretty much at zero. The tool
could not cut that material cleanly away because it was probably
being pushed away from the tool tip. Conclusion is to always machine
through cuts beyond that of the finished part thickness, ensuring
that all material when you flip the part is cut away efficiently and
limits any idiosyncrasies in the material moving.
The lines appear to be about 60 to 75 lines per inch and have
a depth of around .010 to perhaps as much as .020 IN. These are
most noticeable on rounded or areas that have a radius.
I will assume that the witness lines are on a 3D surface. First of
all, 60 to 75 lines per inch (LPI) are very course step overs. At 60
LPI, the step over equals .01666" recurring, and for those working
in mm’s it equates to a step over of .423mm which is really
unacceptable. At 75 LPI, the step over equals .01333" recurring, and
for those working in mm’s it equates to a step over of .338mm which
is also unacceptable. The depth of the grooves are the direct result
of the step over, and is referred to as the cusp height. In many
software packages, you can select step over or cusp height, which
means that the cusp height needs to be set to zero for a mirror
finish, and that setting will automatically calculate the correct
step over to achieve the desired surface finish. Step overs for
really sharp and super clean surfaces should be anywhere from
.0001-.0005" or .0025-.0127mm. Using the conical engraving tools and
ball end mills will not guarantee a super finish either even if the
step over is very tight, due to their cutting geometry. Forget
getting a nice finish at the surface with an engraving tool. A ball
end mill, although a better choice, is still with problems that need
to be addressed. The tip of the ball, does not cut the material
efficiently, but rather rubs it out of the way. This is due to the
fact that the optimum cutting edge on a ball end mill is slightly
off of centre. Therefore whenever the centre of the ball end mill is
engaging material that needs to be removed, it can, and most likely
will, leave witness marks appertaining to its path direction. This is
why the best surface machining in 3D applications are done via 5 axis
because it rotates either the tool or the part into a position that
allows for the optimum cutting edge to engage the material and not
the tip. The best tool for the job, is a flat end mill with corner
radii. Granted, the pieces I machine these days are larger, therefore
I have more room to work with, but they do have miniature end mills
with corner Radii which are called bull nose tools. The beauty of the
bull nose tool, is that from the face of a centre cutting end mill
around the radii and up to the profiling flutes are all optimized
cutting edges which means that regardless of where the tool engages
the material, the cut is efficient. Also, with a bull nose, the step
over will be greatly reduced when compared to ball end mill and still
achieve the desired finish.
Is this type of tool marking inherent to parts machined with a
mill that uses steppers,
You can get the same problems using servos. Although servos are
superior, at this point, the real issues are not fundamentally the
fault of the drive components, but more so, the lack of the clear
understanding of machining strategies.
or could this be solved by using a faster spindle speed and a
slower rate of travel? Or would it take a different tool size
accompanied by a difference in travel lineal travel, do to the size
of the tool serrations on the edges, to me it seems as though a
very small end mill is being used.
Speeds and feeds are important and critical, however, changing those
parameter alone, will not change the fact that the step overs where
too aggressive, and tool geometry was not considered.
Some straight edges are reasonably free from the edge
serrations which lead me to believe that the X-Y steppers are not
quite working to insure a smooth arc. Or that the Tool is being
pushed too fast,
Not a stepper problem for the most part, but due to the fact that
the linear moves are clean, and the arcs are not, points me to the
software. When machining from data that was derived from a solid
model, this is most likely the culprit. Because of system resources
and the amount of computations going on, most software solutions will
default to a low resolution display to speed up redraws and
calculations etc unless otherwise specified. This is fine when you
are working and time is of the essence, however when it is time to
export that file, you had better crank up that resolution because
what you see on screen, will be exactly what is machined. This
flexibility is there for computing power, but also to reduce and
enlarge export file sizes accordingly for specific tasks. You may
e-mail a colleague a file in a low res, because the file will be
smaller, and once he brings it into the native environment on his
side, he can crank up the res either for display purposes or for the
critical part of machining. 2D DXF files generated from a solid model
will export the lines and curves and simply put as point to point. A
circle in a solid model is in fact faceted. The res level will
determine if it has 6 facets at a low res or hundreds at a high res.
These facets are then transposed to the machine and the result is
faceting on a part. What needs to happen here, is in the CAM package,
replace all of the arcs with new clean arcs that are smooth vectors.
The DXF from the solid model are also vectors, but they bring too
much baggage and way too much Circles when looking at
them in point node will most likely show hundreds of points to
reflect that circle. In Type3, we can select that circle and convert
it into a 3 point circle which is all you need to define a circle.
When you have a super clean arc, the code will reflect this cut as a
starting point, an end point, and an R value for a radius move. This
will now be machined as a true arc and not as a point to point linear
move. Even with steppers, this will reflect a huge improvement in the
quality of the surface. With 3D surfaces, well there’s not much you
can do about that, it is what it is. However increasing the res will
most definitely result in better quality machined surfaces.
The originals are done on Ferris Green which would seem to be a
good material since it usually cuts and scrapes pretty clean, so I
just want to find out whether these (rough waxes) are customary or
is this just a case of operator error of trying to hurry,
Sloppy machining.
I realize that tool marks can be a problem because I used to
work for Northrop aviation and spent many many shift hours in
front of Bridgeport and Lagun Milling machines, but back then NC
was just in it's infancy and I've had no real NC or CNC experience
so I'm not really sure of the limitations of a table top system,
The trick is understanding what causes tool marks and how to avoid
them. I manufacture 5 point harnesses for the Aviation and Motor
Sports industries and one part in particular is 2.75" in Diameter. On
the prototype I finished the top surface with a .5" flat end mill
with a .375" step over. The surface was smooth as silk, however to
the eye you could see the evidence of the toolpath. It wasn’t a
problem because they were to be polished anyways. But being an anal
perfectionist I wanted the delivered part to look better. The
conclusion was that I spent $600 on a 3" Mitsubishi face mill that
cut it in one pass and left close to a mirror finish. Because the
tool was larger than the part, there was no step over and therefore
no evidence of a tool of any given diameter being involved with the
cut.
I have been studying EMC and G code and have collected some
great software but I don't know whether to start doing the CADCAM
my own self or keep swearing at the person doing the waxes I'm
having trouble with.
You can continue along the present path and nothing will change,
except for more grief, or you can take the plunge and take care of
the parts yourself. It is apparent to me, that you have the right
thought pattern and the resolve to want to improve on the elements
that are causing you grief which is a 3rd party. I think you know
what you need to do.
I have managed to get MASTERCAM 9, JewelCad, and two other top
shelf programs, I've been looking at Sherline mills, but they only
work with Linux and EMC I'm used to Linux, but I really don't have
the time to write the code, and keep up my production, I'd rather
let the software do it. Does someone know if I can get a control
card and box that operates on a Windows platform and is it
possible to convert a Sherline to servos instead of steppers or are
steppers even the root of the problem? I'm hoping that I can if
necessary find an inexpensive milling machine that will work with
the software that I have accumulated, that's why I'm really curious
about a Sherline, that and the availability of a 4th axis not to
mention the initial price.
Andrew Werby can answer these issues. He knows this stuff inside and
out.
If you need more help, give me a call.
Best Regards.
Neil George
954-572-5829