CFD Online Logo CFD Online URL
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Verification & Validation

Flow over flat plate with chtMultiregionfoam

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

LinkBack Thread Tools Search this Thread Display Modes
Old   August 18, 2021, 07:11
Default Flow over flat plate with chtMultiregionfoam
Join Date: Mar 2021
Posts: 43
Rep Power: 3
Clau.77 is on a distinguished road
Hey guys!

So i have a multiregion case and no analytical or experimental data to compare it to. In order to get a feeling on how fine the grid must be and how many layers i need, i would like to simulate a flow over a heatet plate and compare it to analytical solutions. I was pretty succesful when i tried it for a single region case, but i was wondering if i can do the same for a multiregion case (or if it is sufficient to just do it for single region).

The case is steadyState with a laminar flow.

I managed to simulate the flow over a plate but I am not really satisfied with the outcome (i am looking at the wallheatflux). So i was wondering if I need to use another boundary condition. Fot T i usually use the compressible::turbulentTemperatureCoupledBaffleMix ed and for U "fixedValue uniform (0 0 0)". Are there other boundary conditions I could try for the mappedWall patch?
Clau.77 is offline   Reply With Quote

Old   September 18, 2021, 09:33
Senior Member
Join Date: Sep 2013
Posts: 342
Rep Power: 19
Bloerb will become famous soon enough
That depends what you want to compare your simulation to. For a flat plate there are usually nusselt numbers given (for turbulent flow). Which you can generate from your heat flux. You need to be careful though how the specific paper calculated that number (what reference temperature was choosen). There should be several papers out there with those values.

For purely laminar flow you can calculate the temperature profile in the fluid depending on the boundary condition. This is called the Graetz Problem. Which yields a constant nusselt number after the initial region. There is no analytical solution for a solid region attached to it. The boundary condition of a fixed temperature or a fixed heat flux needs to be applied to the fluids surface. And there are solutions for the temperature profile for both of them. Keep in mind that those start with a fully developed flow profile. You hence need to choose a parabolic inlet profile. There are boundary conditions for that. If you need help setting those up i'll give you an example.
You likely need this boundary condition for heat transfer. Either in the solid or the fluid region (solidThermo/fluidThermo). With either the coefficient mode to specify a htc or heat transfer coefficient at the wall. Or in power or flux mode to specify power in watt or flux in watt/mē at the surface. Here you need to keep in mind that this is specified over the entire surface. Hence the thickness of your 2d mesh is incorporated into that.

        type            externalWallHeatFluxTemperature;
        mode          coefficient;                    
        Ta               uniform 313.15;                       
        h                 uniform 10000;                     
        kappaMethod     solidThermo;                    
        value           $internalField;
On the coupling wall from fluid to solid there is only one boundary condition and that is compressible::turbulentTemperatureCoupledBaffleMix ed.

The problem with a solid region you might face is that you might not get a good paper that lists the thickness of the solid and the type of boundary condition that might apply on it's non coupled surface. If you want to test it though simple choose a thin solid region. It should give you results very close to the pure single region solution.
Bloerb is offline   Reply With Quote


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
Issues on the simulation of high-speed compressible flow within turbomachinery dowlee OpenFOAM Running, Solving & CFD 11 August 6, 2021 07:40
Flat plate analysis in cfx hamed.majeed CFX 14 February 4, 2015 08:07
MRFSimpleFoam simulation flow over flat plate rorating baoaero OpenFOAM Running, Solving & CFD 0 September 17, 2013 22:07
incompressible, 2-D laminar flow over flat plate... varunjain89 Main CFD Forum 3 March 6, 2012 12:13
results for flow past flat plate normal to flow lisa Main CFD Forum 2 August 30, 2005 17:36

All times are GMT -4. The time now is 21:43.