[Sakuyalex]

Hello everyone,


for a formula Student project I had to make a Forced Convection flow. I use STAR-CCM+ 12.02.010 (win64/intel15.0-r8). To train the using of STAR CCM+ I made a simple Model (called “Rechteck”) in a virtual Wind tunnel (called “Block”).


I have been creating a mesh with two regions with one mesh continuum for both. After Assiging the parts to region, I am creating boundary interfaces from the fluid region to the solid. Next Step I right-click on the interface and after clicking on “initialize” got the following Error Message:


Intersecting 1 piece
Intersecting Interface 1 with 14589 faces on partition 0
Interface 1: 0 intersection faces (0% of master area, 0% of slave area)
Added 0 vertices on master side, 0 vertices on slave side.
Original master boundary faces: 12789 Area: 1.9829
Original slave boundary faces: 1800 Area: 18
Verifying interface Interface 1
Warning: no intersections found for interface Interface 1
Update interfaces elapsed time: 0.15801(s)
When I run it the stream goes through my material (which is clear because there is no interface between the regions.) I have a separate physics continua for each region and all of them have the segregated energy models.



Any advice or answers would be appreciated.
PS: The following Advices founded are already tested:


· Star CCM+ Documentation: Examining the Intersection Report
o During the validity check, if no intersections can be found for the two interface boundaries then a warning message is displayed in the output window during the initialization process:
The likely cause in this instance is that you either selected the wrong boundary pairs or did not set the axis of rotation for an axisymmetric case. It's possible that the boundaries are not coincident in space within the specified tolerance.


-> Yes the boundaries are not coincident in space. There is no connection between the wind tunnel boundaries and the model.

· Did you re-generate the mesh after creating the interfaces?
->Yes. Result: Volume Meshing Pipeline Completed: CPU Time: 0.00, Wall Time: 0.00, Memory: 161.62 MB Cells: 18866 Faces: 48556 Vertices: 28186

[HeWeb]

Hi Sakuyalex,

it seems that your setup is wrong. As I understood correctly you created a wind tunnel as a box and additionally the "Rechteck". Thats a typical workflow for OpenFOAM but will not work within Star-CCM+. Lets say CCM+ is a bit more challenging in this kind of simulation. It needs a surface within the wind tunnel region and exactly the same surface within the rechteck region.

First you need to subtract the Rechteck from the wind tunnel, so that you get a wind tunnel region without the Rechteck. Then you can mesh both regions with one or two mesh continuum. After meshing is finished you have to couple the boundary "Rechteck" of the wind tunnel region with the boundary "Rechteck" of the rechteck region.

For a better description have a look to the UserGuide tutorials "conjugate heat transfer" (side 8107)

Hope this helps!

Hendrik

[me3840]

Originally Posted by HeWeb

As I understood correctly you created a wind tunnel as a box and additionally the "Rechteck". Thats a typical workflow for OpenFOAM but will not work within Star-CCM+. Lets say CCM+ is a bit more challenging in this kind of simulation. It needs a surface within the wind tunnel region and exactly the same surface within the rechteck region.

while their setup is in fact incorrect for the reason you describe, I just wanted to say that this setup is equally invalid for OpenFOAM. Both codes operate in the same manner and would require the surface transferring heat to exist in both domains. Both can have the wind tunnel surface and the object itself as separate input parts in the beginning, and both require that the volume mesh respect both of those surfaces in the end.

[Sakuyalex]

Hello everybody
I want to thank everyone for their help.
I especially want to thank Hendrik Weber personally.
Through his explanation I could solve my problem.
The thread can now be closed as successfully closed.