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
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

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?
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
STEP works much better for transferring solid model data from UG to Pro/E. Wildfire can import Parasolid export files from UG.
To get assemblies from UG to show their assembly structure, you must use the external interface. You can do it from within UG, but you have to elect the from file option. You can not select the UG data interactively and get the assembly structure in the IGES file.
If you have solid bodies in UG and are only getting surfaces/quilts in Pro/E then you need to change the export settings in UG to export the solids. By default, I think, UG exports surface data in IGES.
--
Ben


"Jeff Howard" < snipped-for-privacy@mindspring.com> wrote in message
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
: >............... : > 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? :
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
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

become
solid,
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
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..
Da Crew wrote:

Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
<<< "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?
=============================
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Ok, I quickly read through this and I've realized I never did state my version of pro/e.
We are running Wildfire 2.0 build M010, but have received M030, but haven't installed it yet? That's the IT guys' job so I'm not entirely sure.
Yes, turbine airfoils. Pro/e can do a great deal of different types of work. We're not building Lego blocks, as I told our WF2 rep, but we'd like to get into contact w/someone that may have the unique perspective of using WF2 in the turbine airfoil industry specifically with investment casting tooling and ceramic core dies.
Thanks guys, I'll try the suggested methods and let you know...or ask more questions...
The Crew

'extracting'
faces,
etc.
bombed
.igs
tool
The
don't
start
Boundary
better
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

like
using
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.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
(minus the 'remove' thingy).
--
Alex Shishkin



Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
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?
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Polytechforum.com is a website by engineers for engineers. It is not affiliated with any of manufacturers or vendors discussed here. All logos and trade names are the property of their respective owners.