[pemendonc]

Hello, everyone. I'm currently developing a model to simulate the transient heat dissipation on a heated disk brake. My model consists of three domains: the air enclosure, a rotating fluid domain that encapsulates the disc and the solid disc domain.

I defined the inlet air velocity as 7 m/s, the initial temperature of the disc as 200 ºC and applied the angular velocity of 500rpm via "domain motion" on the rotating fluid domain, to simulate the rotation of the brake disc. The other domains were initially set as stationary, with the frame change/mixing model option set to "frozen rotor".

The results I get for the air flow seem to be accurate, but the thermal results are not. I'd expect to see a temperature distribution on the disc that is somewhat symmetric and constant in the tangential direction. It seems that my model cannot properly represent the rotation of the disc. The results I'm attaching to this are 0.13s of simulation, so the temperature difference between regions is small, but it gets larger the more time is simulated and the distribution remais roughlly the same.

I've tried to solve this via a few different approaches: by applying solid motion to the solid domain (the temperature either goes up indefinitely or goes down to 0K), by applying wall velocity of 500 rpm to the inner walls of the rotating domain (doesn't change much) and by applying rotation to the solid domain via "domain motion" (doesn't change much).

I'm now out of ideas. Any help would be much appreciated.

[ghorrocks]

Have you read the FAQ on accuracy? https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F

In your case things to particularly look for are:
* The default convergence conditions may not be accurate enough. Make sure you include imbalances in your convergence criteria, and do a convergence sensitivity sweep to make sure you are converging tight enough.
* Check your mesh is fine enough. You always have to do this.
* Are you sure the Frozen rotor assumption is appropriate here? I suspect you might need to do a full transient model with the transient rotor/stator approach.

[pemendonc]

Originally Posted by ghorrocks

Have you read the FAQ on accuracy? https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F

In your case things to particularly look for are:
* The default convergence conditions may not be accurate enough. Make sure you include imbalances in your convergence criteria, and do a convergence sensitivity sweep to make sure you are converging tight enough.
* Check your mesh is fine enough. You always have to do this.
* Are you sure the Frozen rotor assumption is appropriate here? I suspect you might need to do a full transient model with the transient rotor/stator approach.

Hi, Glenn. Thank you very much for taking the time to answer my question. I'll address the points that you made. In the meantime, I'm open to any other suggestions.

Best regards,

Pedro

[pemendonc]

In case someone has the same issue, the frozen rotor assumption was indeed not adequate for this problem. I ran the model again, this time applying domain motion to the solid domain and changing the "frame change/mixing model" to "transient roto/stator" on both the rotating fluid domain and the solid domain, and the results were much better. I've attached an animation that I made showing the temperature change over time. Thank you so much for the tip, ghorrocks!

Animation: https://imgur.com/a/JbKzlAz