|
Accuracy- The accuracy after using MetaCut
will be exactly what you specify. However it is important to realize
that accuracy starts back in the design stages. Relative to the
machining process, when we speak of accuracy, we usually mean how
accurate relative to the original CAD model. This is easy to calculate.
If we assume that the CAD model is perfect. (it's not). Then there are
two more places for error to be produced before you begin the actual
machining process. The first place for error to be produced is in your
CAM system. You specify the amount of error when you make a toolpath.
This is usually called the "Chordal Deviation" or "tolerance" of the
toolpath. If you keep in mind that virtually all CAM systems produce
toolpaths that represent the curved surfaces of a part as short straight
lines, it is easy to see that here is where the error begins. The idea
is that you produce a path with an "acceptable" error. It would be fair
to say that everything you do to produce a mold has an acceptable error
built into it. There is no such thing as perfect, only close enough.
Your job as a machinist is to make the final part "close enough".
The second place for error to accumulate is in MetaCut. MetaCut must fit
the point to point data with arcs or curves. You specify a tolerance and
MetaCut produces the new entities within the tolerance you specify. You
must keep in mind that the error in MetaCut is added to the previous
error in your CAM system to produce the final total error relative to
the CAD model. If the total acceptable error for your part is .0005",
you need to add the error in the original toolpath to the error in
MetaCut and make sure that the total is under .0005".
This brings up an interesting point. Different CAM systems specify the
tolerance in different ways. There are three primary possibilities as
follows:
1) The tolerance is specified as a single
number but is actually a plus or minus tolerance. In this case if you
specified a tolerance of .0003 your toolpath could go below the
original surface by .0003 and above the original surface by .0003 for
a total error of .0003 + .0003 = .0006".
2) The second method is for the CAM system to specify one
number that represents the total error. In this case a tolerance of
.0003 would allow the toolpath to go below the surface by .00015 and
above the surface by .00015 for a total of .0003". As you can see,
with the same apparent tolerance, this method is actually twice as
accurate as method number one.
3) The third way to specify tolerance in a CAM system is to
allow the user to specify two (2) tolerances. One tolerance represents
the deviation into the surface and the second tolerance represents the
deviation out of the surface. This is often called "in tol" and "out
tol". In this case the user might specify .0002 in tol and .0004 out
tol for a total of .0006" deviation from the original surfaces.
As you can see from the above samples it is important to know which
method your CAM system uses. If you don't know, you do not know just how
accurate you are making your part. MetaCut uses method number one (1).
You specify one number for the tolerance and MetaCut allows the new
entities to deviate from the original point to point information both
inside and outside of the original points.
If you are unsure of the method your CAM system uses, you can probably
find out just by running MetaCut on one of your files. Because your CAM
system data already includes the error you specified, it is nearly
impossible for MetaCut to fit new entities to a tolerance smaller than
you specified in your CAM system. You can take advantage of this fact to
find out what your CAM system does by running the same file many times
in MetaCut using smaller and smaller tolerances. When MetaCut can no
longer fit arcs to the point to point data, you are probably very close
to the tolerance which was specified in the original file. Because you
know how MetaCut's tolerance works and you know that MetaCut can rarely
fit data with more precision than the file it was given. You can
calculate the method used by the original CAM system. Following this
paragraph are two examples.
Example 1- You make a file in your CAM system which uses a
tolerance of .0001". You import the file into MetaCut and try to run
the file at .0001", you find that it does not fit arcs in the places
you expected it to. You open the tolerance in MetaCut up to .0002 and
you find that it fits arcs very well. In this case the CAM system
probably uses method number 1 above. In this case the most appropriate
tolerance to use in MetaCut is just slightly large than the original
tolerance specified in your CAM system.
Example 2- You make a file in your CAM system which uses a
tolerance of .0001". You import the file into MetaCut and run the file
with a tolerance of .0001", you find it fits arcs in all the places
you expect it to. Then you run MetaCut at .00005" inches and find it
seems to be missing some places where you expected it to fit arcs.
Then you try .00006" and all the arcs are back. Your CAM system
probably specifies the tolerance just like method number 2 above. The
tolerance specified in the CAM system is the total deviation from the
original CAD data. In this case, the most appropriate tolerance to run
in MetaCut is just over half the originally specified tolerance.
You should notice from the above examples that the tolerance you run in
MetaCut is usually directly proportional to the tolerance you ran in
your CAM system. The final tolerance in MetaCut is usually one place of
precision greater than the original tolerance in the CAM system, once
you allow for the difference in the method of specifying the tolerance.
Reduction of machining time - You should see a significant
reduction in machining time. The actual decrease in machining time will
vary from part to part and from machine to machine, but reductions in
machining time are typically 15 to 50% percent with high speed controls
and often 200-400% with conventional controls, best of all, because of
the feed control and mode switching in MetaCut, you will see this
reduction in time without adding error to the machining process.
Depending on your current methods you may actually get a more accurate
part even though you are able to make the part in less time.
Finish Quality- Due to the additional feedrate and mode controls
available within MetaCut you should see the surface finish of your
complex shapes get better. Of course, a better surface finish means less
hand polishing, another time intensive part of mold manufacturing. Less
hand polishing means a more accurate part.
The actual increase in surface quality depends on many factors which
include the following list:
-
The construction of your machine tool and the
control on your machine tool. If your machine is an old machine with
an old control you should see very large differences in the quality of
your surface finish. If your machine is a modern high-speed machining
center the improvement in surface quality will be less obvious. (you
will still be able to machine the part in much less time)
-
How well you collected data for your feed control
table.
-
Whether or not you used the exact stop/continuous
mode switch.
-
What tolerance you specified in the CAM system and
in MetaCut. If the total tolerance of your CAM system and MetaCut is
significantly larger than the tolerance you usually use with your CAM
system alone, your surface finish will suffer.
Polishing Time- Just as in finish quality,
there are a number of factors which determine the amount of finishing
time you will need on your parts. If your parts do not require a
'mirror" finish you may be able to eliminate almost all of your
polishing. The actual reduction in polishing times will depend on how
well you set up, understand, and use MetaCut. The better you understand
the factors which go into producing an accurate part, the less polishing
time will be required. Remember, surface finish and reduced polishing
start with accuracy.
Machine Maintenance- This is almost impossible to quantify but
there is a physical difference in the "feel" of the milling machine when
it is running toolpaths optimized by MetaCut. Even on a high-speed
machining center there is a quality of smooth running which can be felt
just by touching the machine while it is running. Also on your machines
which do not have high speed machining capabilities, the mode switching
of MetaCut will prevent a hard "bump" as the machine reaches the end of
one cut and suddenly needs to travel in exactly the opposite direction.
The very nature of a toolpath which has been optimized with MetaCut is
to produce a smoother operation. This is why even a high speed machining
center can achieve a significant decrease in machining time. The
smoother path, allows the machine to maintain a higher average feedrate,
without inducing additional error.
Top
|
