CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   STAR-CCM+ (http://www.cfd-online.com/Forums/star-ccm/)
-   -   Multiple Physics Continua (http://www.cfd-online.com/Forums/star-ccm/87491-multiple-physics-continua.html)

boathead April 21, 2011 06:41

Multiple Physics Continua
 
1 Attachment(s)
I am trying to set up a conjugate heat transfer model (in the case of the attached image, just a simplified version of the main model). The model has 4 separate regions; the solid plate in the middle, the top box, the bottom box and the tube in the middle. Fluid is supposed to flow through up through the bottom box, through the tube and into the top box where there is a crossflow (left to right).

I am trying to incorporate two separate physics continua, one for the top box and one for the bottom box because I need to specifiy different pressure and viscosity boundary conditions at A and B respectively. At both A and B I am using a velocity inlet as my boundary condition which is why I cannot use one physics continuum.

The problem I am having is that, having created all the necessary interfaces between the fluid and solid regions and the fluid to fluid regions (i.e the top and bottom of the tube with the wall of the top and bottom boxes), when I apply physics continuum 1 to the top box and physics continuum 2 to the bottom box and leave the tube without (or with physics 1 or 2) no physics continuum, (depending on which physics continuum is applied to which region) it will change either the interface at the top (highlighted by the red circle) or bottom of the tube from an internal interface to a baffle which means the fluid will not go through it. I cannot even change it from a baffle back to an internal interface which is frustrating!

Is it possible to have two physics continua in such a case and if so what is the best way to get around the baffle issue.

Cheers

alastormoody11 April 25, 2011 04:10

Hi,

One thing you could do is set it to a porous baffle and set the porosity to 1 so it will act like an internal interface. this is hardly an elegant solution but if nothing else works you might want to try this out

boathead April 25, 2011 08:14

I cannot actually change the interface type at all. I have read in the help manual that the internal interface will not work with a different physics continuum either side of it.

abdul099 April 28, 2011 18:09

I suspect, you don't just have to change the interface types, but set up the simulation the right way. It just sounds weird.
First, you don't have to set up four different regions, put all fluid regions in one. You can set several velocity inlets in the same physics continuum. It DOES work!

Second, it's NOT possible to have several regions with different fluid physics continua connected to each other. Create ONE physics continuum and apply it to ALL fluid regions. All of them will have the same fluid, the same properties, are connected to each other and obey to the same physics - so why do you try to set up TWO physics continua???

sebastianh April 29, 2011 06:37

Hi Matt,

you can change the Interface type under the Interfaces main point.
That works in my case. 2 Regions, 2 physic continuums.

It doesn`t work if you change your Interface type under regions.

cheers

alastormoody11 April 29, 2011 09:59

Hi,

Sorry for the late reply.

If during the course of the simulation you want to keep the density and viscosity of the fluid entering from different inlets as the same and different from each other you will need to perform a multiphase simulation though a bit unphysical this is an easier approach.

If you want that the density and the viscosity of your fluid to change with temperature, which is why i presume you are specifying different properties for the same fluid you will need to create a field function and table and change the property with the solution which will a considerably more involved approach.

If what you want is just initial condition to differ you can do that simply by using a field function, which checks the height of your cell and then assigns the value depending on the location of the cell, use the field function in the pressure tab.

Hope this helps

TrII4d December 4, 2011 13:33

Hi,

first: sorry for the late reply (but maybe it helps other users ;-))

you're right, when you say:

I have read in the help manual that the internal interface will not work with a different physics continuum either side of it.

so star ccm+ changes the property of the interface to "baffle" ... and this function does not allow the fluid to go threw the interface

what you can do:

make three regions:

region 1: output/input region with physics 1
region 2: copy of the regions, where the fluit has to flow with physics 1
region 3: orginal of the regions, where the fluit has to flow with physics 2

make interface between boundary of region 1 and boundary of region 2 --> in-place interface (cause of the same physics)
Make interace between region 2 and region 3 --> Heat excahnger interface cause of the different physics and the interface between two regions!

at least, you can translate the region 3 to the left or right. than you can see what happens in the simulation.

you can't create interfaces between boundaries of regions, who have different physics!

so you have to copy one regions, give them the same physics, make interfaces an then create a third regions with other physics.

an interface between two regions with different physics in possible.

greetz


All times are GMT -4. The time now is 14:52.