Altair RISE

A program to recognize and reward our most engaged community members

Nominate Yourself Now!

How to fix the No.of .Boundary layers in Conjugate heat transfer analysis?

Hi ,

I am currently performing a Conjugate Heat Transfer (CHT) analysis (steady-state) using SIMLAB and AcuSolve. The MRF (Multiple Reference Frame) RPM is approximately 20,000, and my CAD model includes a universal motor. Based on this, I estimated the heat source to be around 900 W.

I used a CFD mesh for both the fluid and solid domains, with six boundary layers and a surface mesh fraction of 0.1. The boundary layer mesh type is set to tetra.

After setting up the boundary conditions, I solved the model and reviewed the results. The temperature in the body where the heat source is applied reached 600°C, which is much higher than expected. I then reduced the number of boundary layers to four and ran the simulation again. This time, the temperature in the same region was around 100°C.

This significant difference has left me unsure about how to correctly choose the number of boundary layers.

In simpler cases, such as external flow over a flat plate or internal flow through pipe-like structures, there are standard methods for calculating boundary layer thickness and the first layer height. However, for my current case, I’m unsure how to determine the appropriate boundary layer setup.

Could you please advise on how to select the boundary layer configuration for this type of simulation?

Thanks & Regards,
Siva.

Find more posts tagged with

AcuSolve

HyperMesh CFD

SimLab

Accepted answers

acupro

The boundary layer meshing has a few important parameters - first layer size, layer-to-layer growth ratio, and number of layers. Let's say you want to see the effect of cutting the first layer size in half. If you keep the same layer-to-layer growth ratio (and I like to keep that as a constant - 1.2 to 1.3 generally - but that can also be a sensitivity to study), you may also need to increase the number of layers in order to keep a smooth size transition from the last boundary layer element to the interior elements.

If you also want to keep the aspect ratio similar for that first boundary layer element, you will need to reduce the surface mesh element size.

So what you need to change in the meshing parameters depends on which sensitivity you want to study.

Ovando_RBB

Another method that you can apply is track the output variable of interest (Y) across increasingly finer meshes, where you keep track of the ratio of the element size and number of layers at the boundary (X); there will come a point at which you will be able to interpolate the X-Y function to tell what is an acceptable min. element size and number of layers for you application.

Make sure that the output variable is not just a value at a node or an element, it should be the integral of the total effect at the surface of interest. In that case, I will recommend you to use as on output variable either the film coefficient, drag coefficient, or pressure drop.

All comments

acupro

Did you only change the number of layers - or did you also change the first layer height? Is the growth ratio the same? Did four layers yield a larger size transition from the last boundary layer element to the interior? Is the convergence equivalent? Etc… I've not seen a lot of work on effect of boundary layer meshing parameters on the heat transfer results - but that's certainly a sensitivity one could explore. I have seen mention that heat transfer does perform a bit better with prism/wedge boundary layer elements than with tets.

Sivaprakash_V

I adjusted only the number of boundary-layer (BL) layers. I set the first BL layer height as fraction of mesh size (0.15) size, with 6 & 4 layers, and used a constant growth ratio of 1.2.

My next step will be to mesh the BL using prism cells instead of tetra layers.

Is this approach for the boundary layer correct? If not, how should I proceed instead?

Ovando_RBB

Hi there,

To evaluate the accuracy of your CFD model, you need to perform a mesh sensitivity analysis. This involves running the same simulation with different mesh resolutions while keeping all other parameters constant.

If your output variables (e.g., flow velocity, film coefficient, temperature) show minimal change across increasingly finer meshes, then your model is likely well solved. Nevertheless, if the results differ significantly, especially between the fine and very fine meshes, it suggests that your current mesh is still too coarse to accurately capture the physical phenomena you want to study. In that case, refining the mesh further or adjusting the model setup may be necessary.

ShareShareReply

Sivaprakash_V

Could you please guide me on how to perform a mesh convergence study for CFD analysis? In structural analysis, we usually focus only on mesh size, but I understand that in CFD, additional parameters like the number of boundary layers and the first layer height are also important. I would appreciate your help in understanding how to properly consider these two parameters in the study

acupro

Ovando_RBB

Sivaprakash_V

Thanks for your answers.

Best Regards,

sivaprakash V.