Make:
New Intelli-Max® cutting model precision and
speed optimizations:
Note
All leads must be
defined with quality of "Lead" for the parts to pierce and offset
properly. If you have older files that are not defined this way, then
they may or may not turn out as you expect them to. In this case,
simply change their qualities in Layout as appropriate.
Second generation precision cutting model
For nearly 10 years now, our "old" cutting model has been the best in
the industry for creating precision parts in minimal time. During that
time, this model has experienced incremental tweaks and changes to
provide
slightly better precision. That is what we consider our "first
generation
cutting model." In the meantime, we have launched a huge effort to
expand this model into new areas of prediction. This "second
generation" model
is now implemented in the OMAX Windows 2000 controller.
The cutting model now considers many more parameters, and can predict
things such as taper and surface finish, and has been modified to
improve both speed and precision. The following paragraphs outline some
of the new changes brought about with the new model.
Note: Machineability values of materials are slightly different than
they were. The new values are close enough that most people
will not notice, but they are different. Also, the default materials
database has been changed to reflect these changes. When you install
the software, the old materials database will be backed up, and the new
one will replace it. If you have added a lot of user materials, then
these will be lost (but
preserved in the backup.) These old materials can be recovered by
splicing the databases together using a text editor. Consult the OMAX
Interactive Reference under the Index topic, "Materials database file"
for information on how to do this, if needed.
Super fast Piercing
An updated and much more sophisticated pierce model and method provides
the fastest possible dynamic pierce speed for the given conditions.
Make will use the cutting model to predict the optimal distance and
speed for dynamic piercing for the given part. It will then grow or
shrink the lead-in as appropriate to be the optimal distance without
interfering with other features in the part. If there is not enough
room for the fastest possible pierce, Make will automatically adjust
the speed of motion to compensate. All of this will be automatic, and
without customer intervention. This will greatly speed up nearly all
pierce operations.
Traditionally, dynamic piercing has been considered to
be a relatively slow method of piercing when compared with "wiggle
piercing." This is because it has been difficult to predict the optimal
speed to move the jet to do the fastest pierce—if you guess wrong, you
waste a lot of time. It is also difficult to predict the optimal length
of the pierce move, so that you do not waste time cutting more than you
need to. The OMAX Optimized Dynamic piercing methods change this.
With the OMAX Optimized Dynamic Piercing option
enabled, the software automatically assigns an optimal pierce distance
and speed to each pierce point. If there is not enough room for an
optimal length pierce,
the software will automatically use whatever room it has, and grow or
shrink
the pierce speed accordingly. This results in a faster tool path
without
the need for additional programming—your parts machine faster, and you
will
spend less time programming the tool path.
Make will make the optimal path for you.
(Wiggle piercing is still available for special cases
where it may still offer some advantages, or backwards compatibility.
Wiggle piercing can still be faster than dynamic piercing in the case
where the lead in
is short, and the part is thick. For example, when drilling ¼"
holes in 2" steel, wiggle piercing is the way to go.) In this case, you
can enter in the number of wiggles just like you are used to doing, and
gain a slight edge in speed.
Overrides are also available to disable this feature for special
purposes such as research applications, or to compare time studies with
the "old" method.
If a material is specified as "Brittle", then the lead in length will
not be modified. This allows you to draw the lead in extra long to
allow for cracking away from the actual part.
Note
To take advantage of OMAX Optimized Dynamic Piercing, simply
enter "0" for number of wiggles, and let
Make do the rest.
Quality of “Minimum Taper”
This new cutting Quality tells Make to
slow or speed up the cutting as necessary to provide the minimum amount
of taper (in metals). In most cases, this means that the
cutting speed
will slow down significantly—sometimes to even slower than a Quality of
5. However, in some cases, where "reverse taper" would otherwise occur,
the
cutting speed will be faster. Typically on thick parts the speed is
somewhere
around that of a Quality of 4 or 5, and on thinner parts the speed is
that
of a Quality 5 or slower. In either case, the part will be of higher
tolerance
due to the near elimination of taper.
Although Quality of Minimum Taper is primarily a
precision benefit, there is also a speed benefit in that the programmer
does not have to guess at what feed rate to machine at, and therefore
programming time is reduced, and there is no risk of “guessing” at a
speed that is too slow or fast for the desired result.
Note: It will not necessarily completely
eliminate taper due to the variances in nozzle performance and
other factors that are outside of the control of the cutting model.
(This is why it is called “minimum taper,” and not “zero taper.”)
Note: Quality of Minimum Taper will typically
slow down the part significantly in most cases. However, in some cases
it can speed the part up.
Note: For non-metals, Quality of Minimum taper is
not very
accurate. Also, for best results use a nozzle in good condition,
high quality abrasive, and minimum stand-off. The OMAX Mini-Jet nozzle
is
ideally suited for reducing taper. (For more information on taper,
consult
the OMAX Interactive Reference.)
Tip: For best results, use the OMAX Mini-Jet nozzle.
This nozzle provides the highest precision, since it naturally produces
less taper than other nozzles. Because of this, it often cuts at about
the same speed as larger nozzles when using the "Minimum Taper"
quality. This results in
very significant cost savings due to less abrasive used, less water
used,
less electricity used, and less wear on the pump.
Automatic Corner passing
In many cases, there is no need to slow down for a corner, if you have
room to go past it. This means that for most outside corners, the OMAX
can cut at full speed. The end result is that you have sped up an area
of the part path that would normally be very slow, and you have
increased the
tolerance of the part by avoiding the slight kerf width growth that
would
normally be caused by slowing down. On parts with lots of outside
corners
defined by lines, this can be a huge advantage!
Corner passing allows you to cut thick parts
faster and to a higher tolerance, by cutting past outside corners,
and then coming back. This eliminates the need to slow down the jet to
let the jet lag catch up, resulting in both an increase in speed, and
an increase in precision. (The increase in precision is a result of not
having to slow down so much, which would otherwise cause the kerf width
to grow slightly.) Most customers will mostly notice the increase in
speed, as the increase in precision is minimal.
Corner passing is much faster and requires less
space than corner loops, which is the older "alternate" method.
Corner loops are traditionally used to speed up corner cutting on thick
parts, but they waste a lot of time cutting the scrap material, and
require a lot of room.
Corner passing is set automatically by Make,
so you do not need to program anything special. The corner passing
geometry, as well as jet kickback is optimized for speed and collision
avoidance so that your part does not get marked by a long corner pass.
Currently, corner passing is only calculated for
corners that are generated by two lines, or very shallow arcs. However,
in the future it may be extended to also include corners made from arcs
that come to
a point.
Just as important as knowing where to place corner
passing is knowing where not to do it. Corner passing is not placed in
places where either the corner passing itself or the resulting
kick-back from the jet will interfere with other features in the path.
When in doubt, Make will not use
corner passing, although corners will still benefit from other
improvements in this release.
Corner passing is most effective on parts where the
cutting quality is low and the thickness is high. This is because these
are the kinds of parts that have the most jet lag. For higher cutting
qualities such
as 4, 5, and “minimum taper,” corner passing may or may not offer a
speed
advantage. For this reason, at each corner, it is determined how far
the
corner pass would be, and if this distance is less than a certain
threshold, then corner passing will not be used.
Note: Using corner passing slows down the
computation of the tool offsetting portion of computing the tool path.
The slow down occurs in calculating interference and collision
avoidance between the corner passing geometry, and the rest of the tool
path. In other words, you do
not want to go past the corner and right into another feature of the
part!
This speed decrease is not very noticeable on paths with less than 1000
entities, but on larger paths it is quite significant. For example, on
a
path with 5,000 elements, it may take an additional minute or so to
calculate the tool offset with the corner passing entities. Therefore,
when using
corner passing, it is recommended to keep your tool paths below 5000
elements,
use a fast computer, or break your tool path into several paths.
Note: To use corner passing, (and some of the other
Intelli-Max® enhancements) you must have a tool offset.
If you enter a tool offset of "0," then corner passing will not be
enabled.
* It is possible to disable corner passing for
the case where you intend to keep the “scrap” and the part, such as
when doing artistic inlay work. This is done under "Setup /
Optimizations" from the pull-down menu.
* It is also possible to disable corner passing for a
single corner, while allowing corner passing on other corners by simply
putting a very small radius arc at the tip of the corner.
Advanced Corner Compensation
OMAX has been making sharp, high tolerance corners since 1993. What
is new, however, is that the same high tolerance corner is even faster
than ever through sophisticated advancements in the cutting model. You
will notice that outside corners cut much faster. Inside corners may
cut
slightly slower, but be sharper. Overall, this enhancement is worth a
significant increase in cutting speed and precision on nearly all
parts, but some parts may be slower.
Note: In order to use advanced corner compensation, you must
use a tool offset. If you enter a tool offset of "0", then the
advanced corner compensation will not work be enabled, and you will not
get any benefits in speed or precision over the older releases of the
software.
Other miscellaneous tweaks and
enhancements
In addition to the above, there were dozens of other minor "tweaks"
and enhancements to the cutting model and its implementation. Each by
itself is of little consequence, but all together they add up to
significant time savings or increases in precision per part. For
example:
Lead outs are now shrunk to zero length, or
very short, except in the case where they may enhance the speed or
precision (that is, tangent or nearly tangent to previous corner). This
means less time wasted on the lead-out, as well as less chance of
marking the part as
it tips into the jet.
In the case of a tangent corner lead out, the
jet is now slowed down slightly to prevent it from skipping into the
already cut area, and leaving a tab holding the part to the
original material. This fixes what has otherwise been a slight
annoyance.
Other minor changes and enhancements have been made as
well. Some of these are trade secrets.