CHT webinar homework: PCB-board forced cooling via CHT
Project Link: Tutorial CHT: PCB forced cooling by jousefm | SimScale
Goto ‘Actions’ and ‘make a copy’.
Follow the steps below for setting up the CHT project for forced cooling of a PCB board.
Step-by-Step
Meshing
- In the ‘Mesh Creator’ tab, click on the geometry ‘PCB-board-CHT’
- Then, click on ‘Mesh geometry’ button in the options panel.
- A new mesh operation will be created. Select the last option ‘Hex-dominant parametric’.
- In the properties select ‘Create multiregion mesh’ to ‘True’.
- Now, scroll down to the bottom and click on ‘Save’.
- Once saved, new entries will automatically appear under ‘Geometry primitives’ with recommended values.
Please make sure the BaseMeshBox and Material Point have the following coordinates:
- Next, we will create 2 ‘Mesh refinements’ by clicking on ‘Add mesh refinement’ in the options panel.
- Add a ‘Surface refinement’ by setting up the options as shown below and clicking on ‘save’.
- Add a ‘Feature refinement’ to refine the edges by setting up the options as shown below and clicking on ‘save’.
- Use a ‘Distance’ of 0.005 and ‘Level’ of 2
- Now, click back on ‘Operation-1’ and click on ‘Start’ button to begin the meshing process.
- The process will begin and the status can be viewed in the lower left corner under ‘Job Status’.
- The meshing process will take less than 5 minutes to finish. The mesh will automatically load in the viewer once done.
Simulation Setup
Now to setup the simulation, switch to the ‘Simulation Designer’ tab.
- Click on ‘Create new simulation’ in the options panel, give it a relevant name and click ‘Create’
- Select the ‘Analysis Type’ options as shown to create a ‘Laminar Steady-State’ CHT simulation and click on ‘Save’.
- After saving, the simulation tree will be generated. We will setup the essential entries required for this simulation.
Domain
First is ‘Domain’, where we select the ‘Mesh’ and can define ‘Interfaces’.
- Click on ‘Domain’ and select the available mesh and then on ‘Save’.
- The selected mesh will automatically load in the viewer.
- We do Not need define any custom ‘Interfaces’ as by default all interface surfaces will be considered as ‘Coupled’ thermal type and ‘No-Slip’ momentum types.
Model
Under model comes the ‘Materials’, ‘Initial conditions’ and the ‘Boundary conditions’. We will go through them one by one.
- First, specify the gravity as shown below:
Materials
- Click on ‘Fluid’ and then on ‘Add Fluid material’ in the options panel.
- Scroll down to the bottom and click on ‘Import from material library’
- Select ‘Air’ and click on ‘Save’
- From the ‘Topological Mapping’ list select ‘solid_8_region’ and click ‘Save’ to assign the fluid material to this mesh region.
- Similarly, Click on ‘Solid’ and then on ‘Add Solid material’ in the options panel.
- Scroll down to the bottom and click on ‘Import from material library’
- Select ‘Silicon’ and click on ‘Save’
- From the ‘Topological Mapping’ list select the following entries to assign the solid material to the mesh regions
‘solid_1_region’ .
‘solid_3_region’ .
‘solid_2_region’ .
‘solid_4_region’ .
and click on ‘Save’
- Now follow similar steps to add a new material ‘Tin’ .
- From the ‘Topological Mapping’ list select the following entries to assign the solid material to the mesh regions
‘solid_6_region’ .
‘solid_5_region’ .
‘solid_7_region’ .
and click on ‘Save’
- Follow similar steps to add the last material called ‘ABS’
- Important : for this you need to specify a value under ‘Specie’ for ‘Molar weight’ of 200.
- From the ‘Topological Mapping’ list select the following entries to assign the solid material to the mesh regions
‘solid_0_region’ .
and click on ‘Save’
Initial Conditions
For the ‘Initial Conditions’ , no changes are required and the default values are used.
Boundary Conditions
- Now add the boundary conditions to the setup. In the sub-tree click Boundary Conditions and select Add boundary condition
Capacitors
- Select the Wall under ‘Type’ and specify a temperature of 313K to the ‘No-slip’ wall as shown.
- Select the Pick faces icon (indicated by number 4 in the image), select the faces from the viewer and click on Add selection from viewer. Click Save
Microchips
- Again click the Boundary condition on the sub-tree and add another boundary ‘Microchips’ with temperature wall 343K, as shown below.
- Pick the faces from the viewer and click on Add selection from viewer. Click Save
Transistors-ABS
- Similarly add the next boundary condition ‘Transistors-ABS’ and specify temperature of 333K.
- Pick the faces from the viewer and click on Add selection from viewer. Click Save
Board-casing
- Add a new ‘Wall’ boundary condition for the ‘Board-casing’ and select Set gradient to zero for ‘Temperature’ condition.
- The faces are selected as shown in the following figure, and click on Add selection from viewer. Click Save
Flow-Inlet
- Add a new ‘Velocity Inlet’ boundary condition for ‘Flow-Inlet’ BC. This is defined as Fixed value ‘Velocity’ with a value in the y direction of -0.1 m/s and a fixed temperature of 293K.
- Select the face by clicking and click on Add selection from viewer. Click Save
Outlet
- Add a new boundary condition for ‘Outlet’ BC. Define the ‘Outlet’ condition with Pressure outlet with default value. * * Select the face by clicking and click on Add selection from viewer. Click Save
Simulation Control
- Click on Simulation Control in the sub-tree and enter the end time as 1000 s with time step of 1.
- Click on Details below write control and enter 500. Select the number of cores as 8 and enter 9000 as maximum run time. Click Save
Create New Simulation Run
- Click Simluation Runs on the sub-tree and select Create new run. Ignore the ‘Warning’ which turns up. Click on OK
- Click on Run 1 and then on Start button. This starts computing the simulation run.
- The simulation runs for 30 mins approximately. Once it is done the status changes to Finished. The ‘convergence plot’ is as shown below.
Post-Processing
1- Click on Post-Processor tab on the top of the window (refer number 1).
2- Click on Solution fields and wait for the results to load. (refer number 2).
3- Move the solution to the last time step (1000) as shown in the image below (refer number 3).
4- Hide the outer geometry by clicking the icon next to ‘solid_8_region’ (refer number 4).
5- Select each region shown in number ‘5’ and then change the type to temperature data T [point-data] (refer number 6).
Finally display the scale by clicking the icon (refer number 7).
Congratulations ! you have completed this tutorial.
