CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > Siemens > STAR-CCM+

Error by creating interfaces for Multiple Regions Heat Transfer

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree1Likes
  • 1 Post By Sakuyalex

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 14, 2018, 10:22
Question Error by creating interfaces for Multiple Regions Heat Transfer
  #1
New Member
 
Alexander Unbekannt
Join Date: Mar 2018
Location: Bonn, Germany
Posts: 2
Rep Power: 0
Sakuyalex is on a distinguished road
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
Attached Images
File Type: jpg Representation node.jpg (69.9 KB, 67 views)
File Type: jpg After Initialize.jpg (84.2 KB, 45 views)
File Type: jpg Before Initialize.jpg (76.9 KB, 48 views)

Last edited by Sakuyalex; March 15, 2018 at 04:23.
Sakuyalex is offline   Reply With Quote

Old   March 16, 2018, 12:26
Default
  #2
New Member
 
Hendrik Weber
Join Date: Jan 2018
Location: Stuttgart, Germany
Posts: 7
Rep Power: 7
HeWeb is on a distinguished road
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
HeWeb is offline   Reply With Quote

Old   March 19, 2018, 00:08
Default
  #3
Senior Member
 
Join Date: Nov 2010
Location: USA
Posts: 1,232
Rep Power: 23
me3840 is on a distinguished road
Quote:
Originally Posted by HeWeb View Post
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.
me3840 is offline   Reply With Quote

Old   March 22, 2018, 05:16
Thumbs up Porblem solved
  #4
New Member
 
Alexander Unbekannt
Join Date: Mar 2018
Location: Bonn, Germany
Posts: 2
Rep Power: 0
Sakuyalex is on a distinguished road
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.
HeWeb likes this.
Sakuyalex is offline   Reply With Quote

Reply

Tags
interfaces error, star-ccm+ 12.02.010

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Selecting Heat Transfer Boundary Conditions Hoppe FLUENT 3 July 11, 2016 00:23
Multiphase heat transfer pkladisios CFX 8 June 7, 2016 02:41
Particle Tracking - Heat transfer and temperature mxodio CFX 8 August 7, 2015 13:43
Bondary conditions for heat transfer between two fluid regions buffi OpenFOAM Pre-Processing 1 July 10, 2015 09:21
Convective Heat Transfer - Heat Exchanger Mark CFX 6 November 15, 2004 16:55


All times are GMT -4. The time now is 01:30.