Igs translation and face/surface extraction

Hi group,

We utilize Pro/e (still learning) and CV. We were first told by the Pro/e
outfit that we would be able to call up native UG .prt files in Pro/e. We
have since found that is not true. We only have one seat of UG and there
are no more engineers here that are proficient at it so it has really become
only a way to convert the files for use in Pro/e or CV.

Our problems have been that when the models are brought into Pro/e after
..igs'ing them from UG NX we see the model as only ONE entity, even though
the list of Quilts is long. We cannot seem to find a way to either export
it as surfaces (into Pro/e) or extract the surfaces in Pro/e (which we can
do in UG). When brought up in CV it usually is a surface model, not solid,
but is sometimes missing information. We've tried exporting from UG as an
..igs and as a parasolid, but neither seems more successful in Pro/e.

Anyone know how to extract surfaces (or quilts) in Pro/e?

Thanks,
The Crew

 

...............

Import Feature in the Model Tree?

What list?

What is "extract"?

If you'll "Edit Definition" the import feature you can manipulate (delete,
repair, etc.) individual surfaces.

If you just want a few surfaces for reference without the overhead of all
the surfaces you can (one of a few ways to go about it, I guess) put your
imported part in an assembly with a "reciever" part and copy individual
surfaces.

I'm curious about the Pro/E / UG interoperability. What are your
experiences? Don't have the UG interface module or it doesn't work for
you? What ver Pro/E?

 

: >...............
: > Our problems have been that when the models are
: > brought into Pro/e after .igs'ing them from UG NX
: > we see the model as only ONE entity, ....
:
: Import Feature in the Model Tree?
:
: > ..... even though the list of Quilts is long. ....
:
: What list?

Maybe the list of quilts under the Layer tree.
:
: > We cannot seem to find a way to either export it as
: > surfaces (into Pro/e) or extract the surfaces in Pro/e ......
:
: What is "extract"?
:
I share Jeff's confusion. If I knew what you were trying to do with these
surfaces, I (we) could be more help. There are, in fact, limited ways to work with
imported solids/surfaces. You can use them as they are for 'Merge/cutout'
operations (AutoCAD/UG/Parasolid boolean subtract). Or, you can do Pro/e surface
copy operations; or you can use the imported surfaces for copy geom from other
models ('Insert>Shared data>Copy geometry from other model') which gets you some
independent surfaces to play with. What you need depends on what you are trying to
do with the imported data. Care to share?

David Janes

: If you'll "Edit Definition" the import feature you can manipulate (delete,
: repair, etc.) individual surfaces.
:
: If you just want a few surfaces for reference without the overhead of all
: the surfaces you can (one of a few ways to go about it, I guess) put your
: imported part in an assembly with a "reciever" part and copy individual
: surfaces.
:
: I'm curious about the Pro/E / UG interoperability. What are your
: experiences? Don't have the UG interface module or it doesn't work for
: you? What ver Pro/E?
:

 

In CV when we hand our programmers our geometry to cut (NC program) they
receive it as a solid since that's how we build it. We generally
'piece-meal' the programmers information as we complete it or as they need
it (airfoil blocks here, shrouds there, etc.). In order for the programmers
to be able to utilize the information, they must break it apart, so to
speak. I don't believe CV will cut solid geometry so the programmers must
turn the solids into surfaces. They do so by 'extracting' the faces or
surfaces from the solid. These generally are untrimmed surfaces which the
programmer must then retrim to one another to create a useful surface model
with which to cut. CV will allow extraction of faces, surfaces and even
edges.

Generally when we receive models in engineering from the customers, they are
already surface models, not solids so we don't usually have any problems.
We've tried to call this .igs file up into CV, but it has bombed out on us
or is missing a lot surfaces or other information. Since we are learning
Pro/E I wanted to take this opportunity to try it there. The quilt list IS
in the Layer Tree as mentioned. They all have the same name and highlight
the entire model when selected.

The subject in question is a rework tool. Therefore I only need a small
portion of the original model which has a LOT of information in it. We
thought by 'extracting' only the geometry that we need, any subsequent .igs
conversion would have a greater chance of compatibility and completeness
since the translator is dealing with a considerably smaller file. The tool
we generally use in UG to 'extract' the surfaces does not work with this
model.

When I build a solid in Pro/E I am able to highlight any surface or feature
individually, but not w/this .igs translation. If I were able to 'extract'
the surface, radius or other information in a more precise manner, it would
be helpful.

I apologize if this isn't very clear as I'm still trying to grasp how Pro/E
works and I know less about UG which makes for a frustrating time in trying
to explain all of this and then ask for the help I need when, in fact, I
don't know exactly where I need the help.

If exporting from UG using different modifiers is the key, then we're
willing to try that. If the key is getting a better model from the customer
then we'll start there, but I doubt we'll get very far. By better model I
mean that a UG-native model SHOULD be able to extract it's own geometry, but
this model will not allow it.

Btw, anyone on here have experience using Pro/e in the specific discipline
of jet-engine airfoils and airfoil tooling?

*sigh*

Thanks guys,
The Crew

 

Da Crew,

(These suggestions have been mentioned already but.. I'll add to help)

The best way, imho, is to open a new file and...
Insert/Shared Data/Copy Geometry from Other Model/Open (the imported
iges proe file)/Default (coordinate system)/Surface Refs/Include/Indiv
Surfs or Quilts.. (now you have the surfaces you want)

Otherwise, if you want to keep the data all in the same imported iges
proe file:
Add all the imported surface geometry to one layer, then,
Insert/Surface/Copy the surfaces (or quilts) you want, then Blank the
layer with all the imported surfaces. (now you have surfaces you want)

Good luck..

 

<<< "In CV when we hand our programmers our geometry to cut (NC program)
they receive it as a solid since that's how we build it. We generally
'piece-meal' the programmers information as we complete it or as they need
it (airfoil blocks here, shrouds there, etc.). In order for the
programmers to be able to utilize the information, they must break it
apart, so to speak. I don't believe CV will cut solid geometry so the
programmers must turn the solids into surfaces. They do so by 'extracting'
the faces or surfaces from the solid. These generally are untrimmed
surfaces which the programmer must then retrim to one another to create a
useful surface model with which to cut. CV will allow extraction of faces,
surfaces and even edges." >>>

If I'm following, you can export discrete surface, quilts, curves (?), etc.
from Pro/E. Quilts can be selected from within the export dialog. Curves
probably require a little layer manipulation (I've never done it, but
believe it should be possible).

-------------------

<<< "Generally when we receive models in engineering from the customers,
they are already surface models, not solids so we don't usually have any
problems. We've tried to call this .igs file up into CV, but it has bombed
out on us or is missing a lot surfaces or other information. Since we are
learning Pro/E I wanted to take this opportunity to try it there. The
quilt list IS in the Layer Tree as mentioned. They all have the same name
and highlight the entire model when selected.

The subject in question is a rework tool. Therefore I only need a small
portion of the original model which has a LOT of information in it. We
thought by 'extracting' only the geometry that we need, any subsequent .igs
conversion would have a greater chance of compatibility and completeness
since the translator is dealing with a considerably smaller file. The tool
we generally use in UG to 'extract' the surfaces does not work with this
model." >>>

One way: Set the selection filter to "Geometry". Highlight and select a
surface. Menu: Edit / Copy, then Edit / Paste (or ctrl+C and ctrl+V). The
Copy dashboard will open and you can (I think) select additional chained
surfaces. (There are intricacies with the "selection" process that I don't
want to get into; I don't understand them well enough to explain, but they
can be figured out and there is a tutorial on PTC's site.) Once you have
copied all the required surfaces, export and specify the quilts to be
exported (look for the Quilt button in dialog).

Another, maybe easier way: Put the reference file in an assembly and start
a new part file (in the assy). Go thru the copy routine and just export
the part file (don't have to worry about filtering the exported entities).

---------------

<<< "When I build a solid in Pro/E I am able to highlight any surface or
feature individually, but not w/this .igs translation. If I were able to
'extract' the surface, radius or other information in a more precise
manner, it would be helpful." >>>

You should be able to, I think. When you have trouble selecting something
that you think you should be able to ditch the Smart selection filter and
set it to the type entity you are after.

You can also determine whether import feature surfaces are treated as
surfaces or quilts. Select the Import Feature, Edit Definition. Menu:
Edit / Feature Properties, clear the Join Surfs box. (It's actually a
little more complicated sometimes; you may have to go thru an Edit Boundary
to get the surface out of a quilt, but let's save that for another time if
it's really necessary <g>.)

----------------

<<< "I apologize if this isn't very clear as I'm still trying to grasp how
Pro/E works and I know less about UG which makes for a frustrating time in
trying to explain all of this and then ask for the help I need when, in
fact, I don't know exactly where I need the help.

If exporting from UG using different modifiers is the key, then we're
willing to try that. If the key is getting a better model from the
customer then we'll start there, but I doubt we'll get very far. By better
model I mean that a UG-native model SHOULD be able to extract it's own
geometry, but this model will not allow it." >>>

Shouldn't be any major problems getting what you want, or shouldn't think
so. Holler back if you can't get it figured out. What version Pro/E are
you using (I've missed it if you've said)?

-----------------

<<< "Btw, anyone on here have experience using Pro/e in the specific
discipline of jet-engine airfoils and airfoil tooling?" >>>

Turbine components or airframe? Can't claim to "know" anything about
airfoils, but do occasionally deal with them in the course of doing
airframe structural repairs. I also do some occasional tooling for static
test fixtures, though the only airfoil related one I've done was a winglet
fixture. Whatcha wanna know?

==============================

 

Cool. Can't help ya. Google search for:

aviation OR aerospace turbine tooling pro/e OR pro/engineer

might get you a start. Might also get your sales rep to put out some
feelers at PTC for some contacts. Good luck with it.

 

Through my current employer I've done a good deal of work for Solar Turbines
in San Diego. My stuff has mostly been tool design, but the tooling I do has
to interface to the Solar's parts, which have a lot of various airfoil
shapes. They don't do aircraft engines; their turbines are built for power
generation and oil/gas pumping stations, but it probably doesn't make a lot
of difference from your standpoint.
I won't be able to help you with WF2-specifics: Solar (and, therefore, we)
is on WF still. But it shouldn't make a hell of a lot of difference, either.
For your purposes it would be the best if your Wildfire rep could get you in
touch with people at Solar. However, don't hold your breath: they are
extremely security-paranoid (with good reason). On the other hand, if there
are any software-related questions I can answer without sharing their
designs, I don't see how this will violate our NDA with them.

You can email me at (minus the 'remove'
thingy).

 

Doesn't ProE offer an "add in" modual for a few thousand dollars that
lets you import a UG solid model complet with feature tree?