Step-by-Step Tutorial for Conjugate Heat Transfer (CHT) Webinar


#1

CHT webinar homework: PCB-board forced cooling via CHT

Project Link: https://www.simscale.com/projects/fischer/tutorial_cht-pcb-board_forced_cooling/
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.


'Tutorial CHT: PCB-board forced cooling ' simulation project by fischer
#2

Something is wrong with the feature refinement?!


#3

Hi @cbabua - thanks for reporting this strange behavior. The values for the BaseMeshBox and MaterialPoint should be automatically populated based on the size of the geometry (this was a recent update). However in your case, the coordinates remained the default values so you’ll need to manually add these values before running the meshing operation.


'test cht' simulation project by yrousselet
'CHT test' simulation project by lcltech
#4

Hi @cbabua

I have right now imported the project from the given link at the top and followed the exact mentioned steps for the meshing.

Everything looks good and there are no issues ( Tested it twice ). see below:

I would suggest you give it a retry by importing the tutorial project from the link at the top and follow the exact steps. As Anna mentioned the entries under ‘Geometry primitives’ are automatically assigned the recommended values once you save ( i.e before the Mesh refinements).

Best,
Ali


#5

Why don’t you put this project on the Tutorials tab within help? I found the video by searching on youtube, then later on I found this topic buried in the forums. It would have helped me a lot when first setting up a conjugate study.

Cheers,
Rich


#6

Hi Rich (@rblackburn),

Thanks for this feedback - we’ll look into making this more clear as it does seem that we have our tutorials scattered in multiple locations. One tab would be ideal.

Thanks again,
Anna