Hi All,

I imported a complex CAD geometry created using CATIA in Build. While creating the B-rep for this geometry I got an error message saying there are GAPs between surfaces. I tried to edit them using two options Edit>Surface>Edge match or Edit>Surface>Sew. In some surfaces it worked and in some it didnt (I have too many Gaps due to the geometry's size as well as the complexity). For this, I increased the tolerance in steps and tried to close this Gaps. It worked for most of the gaps. But right now, I am working with a high tolerance of 0.8 mm and there are some surfaces in my geometry whose dimensions are less than 0.8mm. But to close this gaps I had to bring this tolerance to this number. Otherwise it was not working. Now my questions are.

1) Why are this gaps existing when it were not existing when the geometry was created in CATIA. Is it because of the tolerance. I played a lot with the tolerance when importing this geometry (both increase and decrease). But still the gaps exists and in the same location. Any help in this?

2) Now that I am close to creating the B-rep, will I have problem in the meshing of this geometry, since the tolerance is too high (atleast higher than the dimension of some of the surfaces). What can I do in such case. Can I change the global tolerance back to a small number after creating the B-rep? How would his will effect my meshing task ?

Thanks in advance.

Hi Ahmed! well, first of all, do you have the license for import geometrys from other software? You should look at that. I imported a geometry from Pro-E and i had a lot of gaps and that because of the license. CFX it's very tricky in geometrys, the gaps may be due for the tolerance or maybe it's just the way that cfx imported the surface. I worked my self with a tolerance of 1e-5m, so i think that you could lower your's. If you don't want to do that you can extract the edges curves, delete the surface that it's given you problems and make it again. Or if it's a surface surrounded of surfaces you just delete the problem surface and you make it again with CREATE SURFACE EDGE 4EDGE. I hope this will help you out!

With the mashing maybe you could have problems because of the tolerance, I think you should lower your tolerance.

I had same problems when start working with CFX (Build), after many hours wasted in Build (I even made solid body, but have a lot of problems with meshing and that mesh gave erratical results). Finaly I made good mesh inside CATIA (v5 - we use it)...Mesh was imported in Build through Nastran format (that was in CFX 5.5). Now I`m using ICEM and can simply make hexa mesh for that geometry.

Hi deLuther,

I tried to create the mesh with CATIA V5R12 and export the mesh. But I didn't see the export option for the mesh. Normally, it is a global standard to use the term 'EXPORT' for doing such things (I mean, within the CFD/FEM/CAD programs). Is CATIA using someother term? or is it a license problem. If it is a license problem, I should atleast see the term Export somewhere and just I should get a error message saying I dont have license enabled. Then why I was not able to export the mesh from CATIA. Thanks in advance.

In CATIA (we are using V5R11 currently) i used Advanced Meshing Tools. In that workbench there is toolbar named Meshing Methods and last button of that toolbar is Import Mesh\Export Mesh... Of course file in NASTRAN format, in general you have to edit that file for correction of properties and to exchange node declaration part with element declaration. Because elements are written first folowed by nodes what caused error at import.

Thank you very much deLuther. I created the mesh in CATIA and there are just 2 options available for the export. One is a CATIA V4 file and the other says Bulk Data (.dat). Which one is the NASTRAN format? I guess .dat or am I missing more options. Now I tried to import this mesh in CFX-Pre. There was the following error message

ERROR There was a problem importing the mesh from the requested file. The importing process reported the following problem:

Unable to import mesh: No 3D elements imported.

How can I deal with this? Any idea. I guess this is because I created the surface mesh and not 3D mesh. But I thought as it is the case in CFX-build that you create the surface mesh and automatically the 3D elements are written to the output file while writing the same. Any more suggestions?

Thank you once again

Does your mesh have 3D elements? It can be made by filling with tetrahedrons. NASTRAN format is Bulk data.(.dat)

deLther, when you made your geoometry you could create the solid an d mesh it? And the results that the post gave you were erratical? It's that you put in your first message? Because maybe i'm having that probleme and i even known

My application is turbomachinery. When I first buit my mesh and launched solution there was problem with convergence. And in one node at inlet I get Mach number ~200!!! Then I rebuilt my model entirely in CATIA, I use only surfaces, mesh those surfaces and finaly filled that mesh with tetrahedrons. And no problem with solution. I used surfaces to get 2D regions. Because if you trying to mesh solid - you will get only one 2D region that covers entire surface.

Fine! Thank you very much!

Hello deLuther,

Another question. While creating mesh in CATIA, is it usual that I have to create mesh for individual surfaces (I have more than 200 surfaces and doing one by one is painsome). Then, I guess I have to fill the geometry with tetrahedral elements. Once this is done, I have to export this mesh from CATIA and import it to CFX-Pre. Now my main concern is, what is with the domain and subdomains? Because I didnt really define the domain and subdomains for this solid in CFX-Build. My geometry is really complex and bit tricky. Any idea ? Thanks in advance.

Hello, Ahmed,

First, I think, you need some internal faces, that divide your domain... Then if you fill each group of faces with tetrahedrons you will get tetrahedrons with different properties in bulk file... Or you can assign different dummy properties for elements in Patran(Build) or just create different element groups from which CFX-Pre will form different 3D regions. (of course do not forget to check that you 2D regions will be translated correctly).

Regards, deLuther

Thank you very much.

[milabvieira]

Dear all,

I am trying to set up a case, in which I have three cylinders (each one corresponding to a different material), connected to each other and a small internal cylinder inside the whole domain (which will contain the heat source of my simulation).

The problem is that I have generated the mesh in ICEM and when I imported it to CFX-15.0, I get the following ERROR message:


ERROR
There was a problem importing the mesh from the requested file.
The importing process reported the following problem:

Unable to import mesh: No 3D elements imported.



Since now, thank you very much for your help.

Camila

[derz]

Hi all....I think I know why everyone here was getting the "Unable to import mesh: No 3D elements imported."

In ICEM you probably exported the .msh by clicking "Output to CFX"

Therefore, in CFX-Pre, when you import the mesh, make sure you select "ICEM CFD Mesh". Sometimes you see the ".msh" next to the "Fluent Mesh" option and select that instead and that's when you get the error message.

It is a very frustrating problem as the last thing you'd think of doing is clicking the "Files type" box when trying to make it work!!!