2. Create Case
Open SimFlow and create a new case named electronics_cooling
Go to New panel
Provide name electronics_cooling
Click Create Case
3. Import Geometry
4. Imported Geometry Units
The imported geometry is in STL format, which does not store unit information. We need to confirm the unit in which the model was created. In the selection of unit, we can use the Geometry size label, which displays overall size of the model in each direction. In our case, the default unit meter is correct.
To confirm default unit meter, press OK
5. Display Geometry
After loading geometry, it will appear in the graphics window
Click Fit View button to zoom out the geometry
6. Create Geometry - Fan
Add fan geometry to the model. It will be placed above the CPU.
Select Create Box
Change geometry name from box_1 to fan
(double click to edit name and press Enter to confirm)Set the origin and box dimensions
Origin \({\sf [m]}\)0.050.0160.0115
Dimensions \({\sf [m]}\)0.0160.0164e-03
7. Create Face Groups - Fan Inlet
Now rotate the geometry of the model so that we can see the bottom side of the newly created fan. We will now select a face that will be subdivided from the fan as a separate boundary patch by the meshing tool.
Press Ctrl and select this bottom surface of the fan
Click Geometry Faces next to fan
Click Create New Face Group
Click Create Group From 3D Selection
Rename group_1 to inlet
(double click on the group to rename, press Enter to confirm)
8. Create Geometry - Outlet Tool
The last primitive geometry to create is a box that will be used as a tool to extract outlet patch from outer boundaries
Select Create Box
Change geometry name from box_1 to outlet_tool
Set the origin and box dimensions
Origin \({\sf [m]}\)0.08450.04150
Dimensions \({\sf [m]}\)6.5e-039e-038e-03
9. Meshing Parameters - Fan
Since we are going to perform CHT (Conjugate Heat Transfer) simulation, we need to create the mesh for fluid and solid sub-domains. We will specify the mesh parameters for all geometries and using the material point we will choose the subdomain that will be meshed.
Go to Hex Meshing panel
Select fan geometry
Enable Mesh Geometry
Set Refinement to Min 1 Max 3
10. Meshing Parameters - Board
Select board geometry
Enable Mesh Geometry
Set Refinement to Min 2 Max 3
11. Meshing Parameters - CPU
Select cpu geometry
Enable Mesh Geometry
Set Refinement to Min 2 Max 4
12. Base Mesh - Domain
Now, we will define the base mesh. The box geometry determines the background mesh domain.
Go to Base tab
Define the box size
Min \({\sf [m]}\)000
Max \({\sf [m]}\)0.0850.0560.0155Define the number of divisions
Division15105
13. Base Mesh Boundaries
Change boundary type to wall for all base mesh boundaries
14. Solid Mesh - Material Point
In order to create the mesh in the solid region, we will place the material point inside the fan geometry. The resulting mesh will remain only in this region.
Go to Point tab
Specify location inside the CPU box
Material Point0.0580.0245e-04
15. Solid Mesh - Start Meshing
Everything is set up now for the meshing of the solid region
Go to Mesh tab
Press Mesh button to start meshing process
16. Solid Mesh
When the meshing process is finished, the solid region mesh appears on the screen.
17. Solid Mesh - Create Sub-region
Before generating a mesh for the fluid region, you must convert the current mesh into a sub-region. Otherwise, it would be overwritten by the new mesh.
Go to MESH panel
Expand the Options list next to the default region
Select Make sub-region
Enter Region Name to solid
Press OK
18. Solid Mesh - Type
Expand region type options
Select Solid
19. Fluid Mesh - Material Point
Once the solid region is created, we can move the material point to anywhere inside the base mesh, but outside the solid region.
Go to Hex Meshing panel
Go to Point tab
Specify location inside the fluid mesh
Material Point0.0580.0245e-03
20. Fluid Mesh - Start Meshing
Everything is set up now for the meshing of the fluid region
Go to Mesh tab
Press Mesh button to start meshing process
21. Fluid Mesh
The mesh will be displayed in the graphics window
22. Fluid Mesh - Extract Outlet (I)
In the geometry setup, you created outlet_tool . You will now use this box to extract patch from boundary patch
Go to MESH panel
Click Options button next to boundaries patch
Select Extract From option
23. Fluid Mesh - Extract Outlet (II)
Pick outlet_tool from the list
Click Extract
The new patch will appear on the list of boundaries
24. Fluid Mesh - Outlet
Now we have to rename the newly created boundary
Change boundary name from boundaries_in_outlet_tool to outlet
25. Fluid Mesh - Create Sub-region
Now, after you used the Extract tool on the default mesh, you can convert it into a sub-region. It’s important to note that extract operations are no longer available once the mesh is converted.
Expand the Options list next to the default region
Select Make sub-region
Enter Region Name to fluid
Press OK
26. Create Region Interface
Two mesh regions are not coupled until you create a region interface. It will be further used to define which information is exchanged between regions.
Select the cpu in fluid region and the cpu in solid region
(hold CTRL key and select both boundaries)Press Create Region Interface
27. Set Boundary Conditions
Make sure the boundary conditions are as follows
board wall
boundaries wall
fan wall
fan_inlet patch
outlet patch
board wall
28. Select Solver
We will use CHT Multi Region SIMPLE solver. This is a steady state solver that allows modeling of conjugate heat transfer and radiation.
Go to SETUP panel
Pick chtMultiRegionSimpleFoam from the list of available solvers
Select solver
29. Radiation
We will first run a simulation without taking radiative heat transfer into account. However, it is important to set up all radiation model parameters now (these parameters cannot be changed later without resetting simulation).
Go to Radiation panel
Uncheck Enable Radiation
Set Radiation Model to Surface To Surface
Increase the Max Rays number to 3000000
30. Thermophysical Properties of Solid
Now we need to define solid and fluid properties. We will assume that the working fluid is air and the solid is made of aluminum.
Go to Thermo panel
Select solid region
Click Material Database button
Select aluminium material
Click Apply
31. Thermophysical Properties of Fluid (I)
Select fluid region
Click Material Database button
Select air material
Click Apply
32. Thermophysical Properties of Fluid (II)
Set the Equation of State to Incompressible Perfect Gas
33. Turbulence
For turbulence modeling, we will use \(Realizable \; k{-} \varepsilon\) model
Go to Turbulence panel
Select RANS turbulence formulation
Select \(Realizable \; k{-} \varepsilon\) model
34. Solution - Solvers
We will now adjust the solver tolerance threshold of the enthalpy equation in the solid region in order to achieve better convergence
Go to Solution panel
Select h (solid) tab
Expand solver options
Lower solver Tolerance to 1e-08
35. Solution - SIMPLE
To achieve better convergence we will adjust SIMPLE algorithm settings.
Go to the SIMPLE tab
Increase number of Non-Orthogonal Correctors to 2
36. Solution - Relaxation
Go to Relaxation tab
Adjust relaxation coefficients
\(h(solid)\)1
\(p {-} \rho gh\)0.3
\(U\)0.4
\(h\)1
\(\rho\)0.8
\(k\)0.8
\(\varepsilon\)0.8
37. Solution - Limits
Now, we will adjust the limits of temperature fields in order to narrow the convergence space of the solution
Go to Limits tab
Enable Temperature Limits
Adjust minimum and maximum temperature to a reasonable range
\(T_{min}\)290
\(T_{max}\)600
38. Cell Zones
Now set heat source term in the CPU volume. In this tutorial, we assume that only the CPU produces the heat of power of 0.25 W and its volume is about 200 mm 3 :
Go to Cell Zones setup
Enable Source term for all cells in solid
Click Add/Remove in Source Terms
Select h equation
Set explicit source term
h Explicit \({\sf [W/m^3]}\)1250000
39. Boundary Conditions - Inlet (Flow)
Now, we will define the inlets and outlet boundary conditions. On the inlet, we will set constant air inflow.
Go to Boundary Conditions panel
Select fan_inlet boundary
Set the Velocity Inlet character
Set the inlet velocity
U Reference Value \({\sf [m/s]}\)0.1
40. Boundary Conditions - Fluid Region (Thermal)
We will now enable radiation coupling on the fluid side of the interface
Click on cpu in fluid
Switch to Thermal tab
Select Coupled Temperature and Radiation type
41. Boundary Conditions - Solid Region (Thermal)
Next, enable radiation coupling on the solid side of the interface
Select cpu in solid
Select Coupled Temperature and Radiation type
42. Run - Time Control
Go to Run panel
Set Number of Iterations to 800
Click Run Simulation button
Estimated computation time: 10 minutes
43. Residuals
Monitor convergence process under Residuals tab
44. Start Postprocessing - ParaView
Start ParaView software to display results
Go to Postprocessing panel
Start ParaView
45. ParaView - Load Results
Select electronics_cooling.foam
Click Apply to load results
Click Last Frame to select the latest result set
After loading results they will be shown in the 3D graphic window
46. ParaView - Display Temperature Contour (I)
We will now plot the temperature contour on the circuit board again. We will use the same scale, so the differences in results are more evident
Select the followings mesh regions
fluid/board
fluid/cpu
fluid/fan
fluid/fan_inlet
fluid/outlet
solid/board
solid/cpu
solid/internalMesh
(you can check Mesh Regions to select all regions and uncheck others: fluid/boundaries and fluid/internalMesh )Click Apply
Select contour coloring variable to T
Click Rescale to Data Range
47. ParaView - Display Temperature Contour (II)
Results are displayed in the graphics window. Note that the maximum temperature in the domain is 360 K.
48. Radiation Setup
We will now enable the radiation equation in our simulation. To do this, close Paraview and go back to SimFlow
Go to Radiation panel
Check Enable Radiation
49. Start Simulation with Radiation
The case is set up. We will increase the number of iterations and run the simulation
Go to Run panel
Set Number of Iterations to 2000
Click Continue Simulation button
Estimated computation time: 20 minutes
50. Residuals (II)
Monitor convergence process under Residuals tab
51. ParaView - Start Postprocessing (with Radiation)
Start ParaView software to display results
Go to Postprocessing panel
Start ParaView
52. ParaView - Load Results (with Radiation)
Select electronics_cooling.foam
Click Apply to load results
Click Last Frame to select the latest result set
After loading results they will be shown in the 3D graphic window
53. ParaView - Display Temperature Contour (with Radiation) (I)
You will now plot the temperature contour on the circuit board again. You will use the same scale, so the differences in results are more evident
Select the followings mesh regions
fluid/board
fluid/cpu
fluid/fan
fluid/fan_inlet
fluid/outlet
solid/board
solid/cpu
solid/internalMesh
(you can check Mesh Regions to select all regions and uncheck others: fluid/boundaries and fluid/internalMesh )Click Apply
Select contour coloring variable to T
Select Rescale to Custom Data Range
Set minimum and maximum value
Min 300 Max 360Click Rescale
54. ParaView - Display Temperature Contour (with Radiation) (II)
Results are displayed in the graphics window. Note that in this case, the maximum temperature in the domain is 343 K, which is 17 K lower than in the previous simulation.
55. ParaView - Radiative Heat Flux (I)
Radiation plays an important role in this scenario. Therefore, our last task will be to display radiative heat flux mapped on the geometry
Set contour coloring variable to qr(partial)
Uncheck mesh regions solid/rPi2_CPU and solid/internalMesh
Click Apply
56. ParaView - Radiative Heat Flux (II)
Results are displayed in the graphics window.
| Note that this tutorial is meant only to demonstrate capabilities of the software and not to solve the problem in the best possible way. Therefore, some assumptions are taken to keep case setup time and computational time low. In particular, to refine the model, one could in first place consider setting more suitable emissivity coefficients for materials used. |
