User Guide: Natural Convection
Firstly, the geometry needs to be ‘CFD ready’
The solid volumes should be non-overlapping and should all be touching each other. More specific preparation details are explained here: Cad Preparation.
Basic recommended geometry checks:
- Ensure that the imported geometry consists of Solid parts and not sheet/surface elements.
- Remove any small fillets or faces which are insignificant for the analysis.
This is a simple LED on a heatsink. It will be tested floating in the air and so will only have natural convection to lose heat.
Reference project here
Once the model is uploaded to SimScale, a fluid domain around the Heat sink should be created to analyse the flow characteristics. This can be done using the “Enclosure” operation under “Geometry Operations” as shown in the picture.
The video here shows how to perform the Fluid Volume extraction/ Enclosure using SimScale
The “Enclosure” option allows the user to set the dimensions of the Fluid volume. To complete this operation, we need to pick a “Seed Face”. A Seed face can be any face of the Heat sink. Picking just one face is enough for this purpose.
Please remember to switch on the “Keep existing parts” option, or the solid parts will not be retained.
The enclosure needs to be large enough to avoid artificially accelerating the air around the sides. These are the minimum dimensions:
Once the dimensions are defined, click “Start” to build the enclosure.
If the enclosure option is not used, the model would need to be ‘Imprinted’ so that all solid components are connected for conduction. This is also in the same menu.
Use the “Hex-Dominant (only-CFD)” mesh in this case. This is the most automated approach and is usually the best starting point.
Start with a ‘Coarse’ mesh. Finer can also be tested later
16 processors or fewer would be sufficient for the model shown.
Once when the mesh is complete, open the Meshing log and scroll down to the last few lines. If there is an error, it is likely that some interfaces are missing between materials. At this point, it might be sensible to reach out to support for assistance.
Ideally, all interfaces will be resolved, as shown here:
- Create a new simulation and select the “Conjugate Heat Transfer” as analysis type.
- Then select the “Turbulence Model” to “K-omega-SST”
- Set the acceleration due to gravity (0,0,-9.81) for example
- In the Materials option, add both “Fluids” (generally air or water) and “Solids” (generally for LEDs – PCB, Epoxy, aluminium etc)
- To assign materials inside the Enclosure -> Right click to bring up the menu to hide volumes
Here is a short video on how to assign Materials to different parts of the model.
In the “Initial conditions”, set the ambient temperature and pressure (101325 Pa)
Supported in the air (like most LED tests)
For the general LED case, which is not sitting on the ground these boundary conditions are set:
- Bottom Face
- Velocity = Pressure inlet velocity
- Modified Pressure = Total pressure 101325 Pa
- Temperature = inlet-outlet – ambient
- Top Face
- Custom and assign the ambient temperature. Everything else remains as default
- Side Walls
- Custom and same conditions as Top Face, except the velocity which needs to be ‘Pressure inlet velocity’
For a unit that is sitting on the ground. We would use these conditions instead:
- Bottom Face
- Top Face
- Side Walls
Assign Volumetric Heat Loads
Advanced Concepts -> Power Sources -> Absolute power source.
Select each volume that will have a heat load and assign a power to it. If multiple volumes are selected, the same power will be applied to each.
It is advisable to set a “Result control” item, to monitor convergence during the simulation.
- Select Result control -> Area average -> then assign some critical faces or points to dynamically monitor the variables during the simulation. Here is an example of what that might look like:
The default values should be suitable
- Change the end time to 2000.
- The Write interval should be the same as the end time to write out the last step results
- To save and view intermediate results, this can be lowered and the results can be viewed during the run
- It is not recommended to save out too many results, maybe 2-5 for a simulation
- Set the “Maximum runtime” to a higher value (10,000 is sensible) – this means that the simulation will run for 10000 seconds and then it will get stopped automatically by the solver (even if the solution is not converged)
- Now create a new “Simulation Run”
- There is usually a warning that certain surfaces will be set to wall boundary condition – this means that the unassigned faces will be set to walls and is totally normal
Results for this sample case can be directly accessed here.
There is a short guide on using our online Post Processor here.