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solid3ddesigns
Guest
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 Posted:
Fri Sep 24, 2004 4:23 am Post subject:
Component face references in assembly |
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I know you can create a part within an asembly and reference faces
from other components to aid creating a new part. Is there a way to
then break the link from the reference faces without having to
redefine the sketch of the new component ?
In Inventor this is called "adaptivity" and you can switch the
"adaptivity off once you have referenced the faces etc. Is there a
similar tool in ProE WF2 ?
Please let's not start a Inventor Vs ProE debate!
Thanks in advance,
HB
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Alex Sh.
Guest
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| Posted:
Fri Sep 24, 2004 7:15 am Post subject:
Re: Component face references in assembly |
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"solid3ddesigns" <solid3ddesigns@yahoo.com> wrote in message
news:f6e59bcc.0409231623.72fc8fb3@posting.google.com...
| Quote: | I know you can create a part within an asembly and reference faces
from other components to aid creating a new part. Is there a way to
then break the link from the reference faces without having to
redefine the sketch of the new component ?
In Inventor this is called "adaptivity" and you can switch the
"adaptivity off once you have referenced the faces etc. Is there a
similar tool in ProE WF2 ?
Please let's not start a Inventor Vs ProE debate!
Thanks in advance,
HB
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No, I don't think there is any other way to do this in Pro/E than to go and
redefine the sketch (in Wildfire, right-click on the feature and pick 'Edit
Definition' from the RMB menu). Once you are back in the sketch, delete all
references to the external geometry and you are done.
As a matter of fact, you can delete the external references right after you
have created the sketch, before you even exit the sketcher.
Of course, your new feature will no longer be driven by the external
geometry after that.
--
Alex Shishkin |
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Jeff Howard
Guest
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| Posted:
Fri Sep 24, 2004 10:13 am Post subject:
Re: Component face references in assembly |
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| Quote: | I know you can create a part within an asembly and reference.....
In Inventor this is called "adaptivity" and you can switch the ...
....similar tool in ProE WF2 ?
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To add to what Alex has said and, hopefully, not confuse the issues too
much....
There are ways, but differences. The whole philosophy is a bit different.
You'd do well to just "play" with it to get a feel for what's going on.
You can project references (Sketch reference collector) and you can project
geometry with the Use Edge tool (references are created automatically and
can be seen and deleted with the sketch reference collector; Menu: Sketch /
References at any time you are in Sketcher mode). You can also delete,
trim, extend the "solid" (vs. construction or reference) curves without
deleting the reference geometry. Deleting the underlying references will
create dimensions and constraints which you can modify or simply "make
strong".
Deleting reference geometry is similar to Break Link. There is not really
a corollary to turning off Adaptivity. In IV it's recommended to turn
Adaptivity off to avoid a performance hit (?) when you aren't actually
using it to drive changes. In Pro/E you just leave the references alone
and go on about your business unless you decide you don't want changes in
the parent to drive the child.
There are a few other differences you might want to get familiar with. If
you reference an edge that is later "consumed" by another feature (fillet,
chamfer, etc.) the reference remains unaffected (e.g. the child isn't
orphaned). If something does become orphaned (the parent is deleted), use
the reference collector to delete the reference. You can query
dependencies via Info / Parent / Child (handy when you can't remember
what's driving what or to get an idea what the ramifications of making a
change might be).
I'm not sure I understand the concepts in either program well enough to be
really concise about the differences, and, like I said, it would be a good
idea to do some experimentation to get a feel for them.
| Quote: | Please let's not start a Inventor Vs ProE debate!
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Debate takes two. Ignore what you want. 8~)
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