CFD Online Discussion Forums

CFD Online Discussion Forums (
-   STAR-CCM+ (
-   -   Porous Region within Open Air "Wind Tunnel" Region Interfacing (

pkirchner December 15, 2011 17:38

Porous Region within Open Air "Wind Tunnel" Region Interfacing
1 Attachment(s)
Hello there. My University just got Star+ccm, and no one's too experienced yet. I'm trying to determine my flow rate through a radiator by setting it to a porous region within my current wind tunnel region. The radiator is mounted on the side on the side of the vehicle in a sidepod...however I have yet to implement the sidepod into the simulation...wanting get the pressure drop across the radiator set first.
So far I've followed the "porous media flow" to set up my simulation.
I started by importing the part all from one pro e file....assigned the wheels, body and all sides of the original "block" to Region 1, set as air.
Velocity- Inlet (16 m/s)
Pressure- Outlet
Walls- Symmetry Planes
I Split the radiator into 3 boundaries, inlet, outlet and walls...I assigned them to a new porous region. Both the regions have their own mesh, and physics continuum. The volumetric control for region 1 is a smaller block around the vehicle. The volumetric control for the porous region is set as the radiator.
Here is where I am lost... I know i need to interface the 2 together somehow, but am not exactly sure how to go about it...setting interface...or splitting by topology or non-contiguous...
Whenever I run the simulation, the body and wheels are ignored as if they are not their, and the radiator that was set to a porous.
The velocity vectors are approaching the body at an angle, while the inlet is perpendicular...
I'm really sorry for the long post, just trying to get everything in there. I truly appreciate any input...can provide summary report if anyone has experience with this? :)

pkirchner December 16, 2011 11:54

I'm pretty sure I need to create interface between the 2 regions. I've done a split by patch on the initial block to Inlet, Outlet, Walls, and Floor....I also then done the same to the radiator. There is one boundary per part surface, so i've created an interface for the inlets, outlets, walls and floor. Now I'm stuck a bit again. Did I need to split the radiator by patch to create a different boundary for each surface in order to create the interface, or is there a different method. I am unable to generate a mesh on my new simulation....getting a (Error in surface mesh of region air: no triangles in surface)............any input? probably due to my boundaries?

Ooooh, also. Since I have 2, the air....and the other the radiator. Do I need to set the radiator to a boundary under my air region, or when I interface will the region be subtracted from my air volume? Sorry for more info, just stuck.

pkirchner January 2, 2012 11:32

Bump. Still unable to figure it out, have a professor taking a look at it, but no luck so far. Any help is greatly appreciated. Thanks guys.

abdul099 January 2, 2012 21:43

You need to perform some boolean operations to create two bodies: One block-shaped domain (wind tunnel) of which the radiator and all solids are subtracted, and the radiator (could be used like it was imported). You need to do this, ccm+ will not do any boolean operations while interfacing, since there's no almighty sorcerer inside your machine.
The resulting bodies will be input parts for the regions.

Next point: As soon as you hit the "initialize meshing" button or performed a surface or volume mesh, the geometry from the parts level will be transformed to an initial surface. This initial surface will not change anymore, therefore any change done to the radiator on parts level will not effect the initial surface - therefore some boundaries of the radiator could empty when you did something after initialising meshing.
Delete the initial surface representation and try again.

pkirchner January 6, 2012 10:48

Got it. Thanks so much, I'm sure I'll be asking more questions once I get further along in the simulation.

pkirchner January 6, 2012 14:39

1 Attachment(s)
Got the air to pass through the radiator with a pressure drop. I am now trying to input my pressure drop polynomial as a function of velocity into the porous internal resistance which is in (kg/m^4). Does anyone have any tips to do so?

Also...the air is passing through the radiator as if it has no internal geometry...without drawing tubes and fins (which would be too fine of a mesh for my computing setup) is there anyway I can set the porous radiator to an inlet (front face), outlet (rear face), and solid impenetrable sides?

Also...trying no measure mass flow rate through radiator only. Any tutorials, or help menus anyone can direct me to do so? Seems simple, I just can't find it.
I appreciate any help guys. Thanks.

ping January 10, 2012 06:42

use excel to fit a 2nd order polynomial (ie parabola) to your data then get the curves equation and use these as your porous alpha and beta coefs. read the help in Help and Tutorials on how to set coefs.

to prevent flow in other directions within radiator set the coefs 3-4 orders of magnitude higher than the above ones. also have baffle interfaces on the non-flow surfaces of the radiator

mass flow through radiator - create a mass flow report with either the front or rear interface as the part to report on.

ping January 12, 2012 00:21

back to basics since you sent a private message and this should be shared online:
you did not understand the good advice of abdul above, so i will spell it out in more detail:
- in simplistic geometric detail, you need a small box (ie a radiator) inside a larger box (outside fluid domain).
- so in 3D-CAD make the large box
then the small box, but DONT merge the solid bodies - you now have two bodies
duplicate the small body (right click on body...)
subtract the second small box from the large box (boolean operation)
now you still have two bodies, but the big one has been hollowed out
hide the big body and rename the faces of the small body (eg sb-in, sb-out, sb-wall1, sb-wall2 etc)
hide the small body and unhide the large body. hide some of its outer walls so you can see the hollowed out inner walls, then rename these as lb-sb-in, lb-sb-out, lb-sb-wall1 etc so the naming matches the naming used on the small box
unhide all bodies and faces, then on the large body rename one face as inlet and one opposite as outlet
- close 3D-CAD, create parts of the CAD
- create regions from the parts, being carefull to retain the two parts as separate regions and all surfaces as separate boundaries
- you will now have two regions with interfaces connecting them. change the interface types of the inner wall interfaces to baffle type
- mesh and run
n.b. up in CAD you could rename all the inner walls to just one name since there is no reason to have them as separate boundaries and interfaces in most applications.
once you have done and fully understood this exercise, you should be able to tackle more complex geometry.

pkirchner January 12, 2012 19:32

Thanks! Got it now. I understood abdul's post, just didn't duplicate the radiator and do the boolean subtract using the second rad. Thanks for putting up with my lack of experience. I'll have to put a good writeup if anyone else has the problem in ze future.

abdul099 January 17, 2012 20:45

It depends on the version and your specific approach whether you need to duplicate the radiator. I'm usually doing geometry preparation on part level with pretty new versions (currently v6.06). So I don't need to duplicate a body since the original bodies are preserved. This is different when using older versions or doing some operations on CAD part level.
Sorry for causing any confusion...

VIMeerkat March 27, 2014 20:10

Hi, I am literally stuck on the exact same problem as you, any chance you can send that write up?

If you could get back to me ASAP that would brilliant :)

Thank you!

All times are GMT -4. The time now is 13:05.