I have the answer for the reference pattern issue:
It seems that Proe can't distinguish which pattern to reference if you
have more than one pattern in the same places, so you have to make
certain your reference pattern references exactly the same pattern or
all instances will end up on top of each other. The responses I got
follow:
The problem with reference patterns is that ProE has difficulty with the
reference pattern if the feature or component you wish to reference
pattern has references to multiple other patterns.
ProE expects just one patterned reference but if there are more ProE
places all the instances of the reference pattern on top of each other.
For instance, you placed a component with insert in a patterned hole and
a mate to the top surface, but you oriented it to a datum plane which
also happens to be patterned.
If you then wish to reference pattern the component ProE does not know
which pattern to choose as a reference and consequently places all
instances on top of each other.
I've mentioned this to PTC on several occasions. We need control over
the references you wish to use as a reference pattern.
Ideally would be that we can just choose any pattern to use as a
reference instead of one of the references of the first feature or
component.
It's great that since WF4 we can also disable instances of reference
patterns, but the ability to choose or change the reference pattern to
follow, regardless of the references of the first feature or component,
is the one thing that would make it complete.
So send in those enhancements requests and probably one day we will see
such an option.
We do quite a few carousels in our instruments so it's important to do
it right to avoid problems. For example, a carousel may have 24
positions with bearings, gears, etc. The first feature might be a bore
for a bearing, the second feature for that location creates snap ring
grooves for the bearing. The snap ring groove feature only uses the bore
geometry such as axis, edges, as references. This will allow the pattern
to be created correctly. HTH.
I've had the same problem many times and have not found a solution, only
a workaround. You can make some offset datums and hang the cuts on them,
and then group the new datums and cuts in a local group. You can then
pattern the local group. It does add some feature overhead to the model,
but I'd rather have overhead than not be able to finish a model.
I've found that the only time this has happened to me, it's because I've
used constraints that reference two (or more) different patterns. Said
patterns may be identical, but Pro/E doesn't understand that and doesn't
know which pattern to reference.
For example, maybe I've assembled a washer to a patterned hole, and
reference-patterned it to that hole. Then, when I assemble a screw, I
insert it into the hole and mate the underside of its head to the top
surface of the washer. If I try to reference-pattern the screw, Pro
doesn't know whether to use the hole pattern or the washer pattern as a
reference. Since I realized this and started making sure I only
constrained to one patterned feature/component, I have not had this
issue.
I usually see this when I accidentally select references from two
different patterns for my dimension scheme.
Make sure that the parents are only from the original pattern and you
will probably be OK.
Thanks to everyone who responded.
Ken Sauter
DRS Reconnaissance Surveillance and Target Acquisition
Infrared Technologies Division
PO Box 740188
Dallas, TX 75374
214-860-6826
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