Import IGES As Solid???

Dear All:


I have an IGES file that I can easily import into Pro. The problem is that it comes in as a hollow shell instead of a solid. I need to import this in as a solid for modelling purposes. Any help is appreciated.\


I have tried some of the random bits of advice I found via search already such as


ntf3d_in_close_open_boundaries yes


intf3d_in_enable_layer_join yes


intf_in_external_accuracy yes


intf_in_keep_high_deg_bspl_srfs yes


I have also opened the file in word pad in order to find the model accuracy to no avail.

Let me add just a little more information.... When I open the IGES file directly in ANSYS, I get a perfect solid, just what I need... The problem comes when I open the model in Pro to add additional Pro components to the assembly and then import into ANSYS - it only sees a shell... Any help out there please???

Yet another piece of the puzzle... If I import the IGES file, add some pro parts to the assembly, then save as IGES again, it opens fine in ANSYS....

IGES is a surface format and contains no solid information. When Pro/E imports an IGES file, it will attempt to 'solidify' the resulting surface IF the surface quilt is 'water-tight'. If it is not, then it will remain a surface.


If you desire not to have the IGES auto-solidified, then you can redefine the import feature and turn off the solidify option.


If your IGES surfaces are being imported and are not automatically solidifying, you could always try manually applying the 'solidify' feature to the quilt. However, the problem may be that there is a small gap in your surfaces that is preventing this. Try working in wireframe mode and looking for one-sided edges (yellow vs. purple). I much prefer to use the Pre-Wildfire color scheme for this since it's hard to distiguish 2-sided edges from 1-sided edges in the new scheme (purple vs. purple???).


-Brian

maesoph,


If you have Import Data Doctor, you may want to check out these links:


[url]http://products.engineering.com/mechanical/software/p00309/d ownloads.htm[/url]


http://www.ptc.com/cs/cs_23/howto/dtr2145/dtr2145.htm


[url]http://www.ptc.com/go/wildfire/learn/interfacing_other/index .htm[/url]


<A href="http://www.ptc.com/appserver/wcms/events/series.jsp?&im_dbkey=11442&icg_dbkey=141Check" target="_blank"> [url]http://www.ptc.com/appserver/wcms/events/series.jsp?&im_ dbkey=11442&icg_dbkey=141[/url]
(Check</A> out the Data Repair webcasts...one is being held tomorrow.)

I've had this issuewith IGES parts imported intoPro/E 2001. The following has worked for me to change them from surfaces to solid:


Redefine the import feature.
Heal Geometry.
Automatic.
All Surfs.
Compute.
Accept..
Attributes.
Make Solid.
Done/Return.


If that doesn't work then there may be some gaps in the surfaces. Try this instead:


Redefine the import feature.
Heal Geometry.
Manual.
Zip gaps.
Auto Select.
Zip gaps.
Attributes.
Make Solid.
Done/Return.


Hope that helps.

Maesoph,


If you have permission from your boss I don't mind looking at it to see if I could convert it.


I use Import Data Doctor quite a bit in my job, we get iges file all the time that need


to be fixed.


Email it to my account linked to this forum but again, as long as you have permission to do so.


Brian

Just as a follow up, I found 2 ways around this problem...


1. Got a STEP file and it imported fine and went forward normally from there.


2. Import the IGES file into the assembly in Pro, add some more pro parts to the assembly, then save as IGES again.Open the exported IGESassembly in ANSYS and it works fine.


Mike

Hi


After redefine the import feature sometime help,


if you set accuracy to 0,01.


Sometime help, ifyou set only accuracy to 0,01


Look there. Maybe help


http://www.pro-des.com/iges.htm


http://www.transcendata.com/cadfix.htm


Good luck