I am using Autodesk simulation CFD 2013 to simulate the naturual air convection of heat sink.
i drew the model in solidworks and imported to the cfd UI, with no problem. simulation and practical results are comparable for heat sink fins, mounted perpendicular to the earths surface.
but the real problem arises, if the fins are inclined to an angle, the simulation results becomes too bad, in other words, the results are crazy.
boundry condition i use are, pressure 0 Pa, on both sides of the air volume and temperature on the lower side of the air volume, the chimney effect. Heat power is given to the surface of the heat sink, where i have made a small extrution to make provision as a heat source. air is set to variable air and also the gravity is assigned. i solve it through mixed length turbulance. meshing is set to automatic meshing. I have the practical results of the same design, I would like to optimize the design. but the practical results and the simulation results are like railway line, they arent coming together. I dont know where am i making mistake.
Practical result is 145 deg C but the suimulation result are somewhere in the range of 3000 degree C. do i need to add some more boundrz condition??..
Kindly help me and thanks for your time.
Solved! Go to Solution.
Confirm that Air is set to [Variable] vs [Fixed]
That is the number one cause of Natural Convection cases producing astronimical temperatures.
Other than that, With Automatic meshing you still have the ability to adjust and refine the mesh. Be sure that the mesh in and around the fins are tight enough to capture the flowfield.
THanks for your time and suggestions.
I made refined the mesh.. temperture is now similar to the experimental results. The result is not converging.. for the first 120 iterations (approximate number), system is stable and the temperature is going good. but later the temperature, pressure and velocity become unstable.. like, they are shooting up and down and never converge.. what could be the reason?..
This can be similiar. Where is the solution going unstable? You could still have a coarse mesh in areas that contribute to the instability.
With natural convection the domain just above the heated components will generate a plume of subtle densivty variation. This plume which helps drive the flow needs to have sufficient refinement to stay stable.
Thanks for the reply..
To be honest, I dont know how to find, where the instability occcurs.. i am not a trained CFD engineer.... I generally loook at the output bar, if the temperature is somewhat linear..
For mesh settings, I had given, volume growth rate and surface growth rate to 1.05. I had just refined the mesh of the heatsink by sliding the bar. I think, your pointing out the mesh settings for air volume.. did i understood you correctly?.
If the solution is oscillating notably (in the convergence monitor) that will be a reflection of the actual resutls having some oscillation within them.
To find some of this within the model you can use an ISO Surface (with vetcors turned on) and look for thsoe areas.
For example, if we ahve higher than expected velocities, or temperatures we can use the ISO surface to look and find the highest temperature in the domain. Once we know where it is we can use an Cut Plane to look at the mesh quality in that area.
Some of the oscillations can be due to the mesh above the heatsink. As the heatsink tries to dissipate the heat you will get a plume of warm air vertically off the components. In many cases the area in the fluid vertically above the heated components may need refinement, this is typically done with a mesh refinement region to capture the plume and how it develops.
The Volume / Surface Growth rate are methods of impacting the mesh globally. At times you may not need a global setting of 1.05, but selective refinement (using the slider bar) or with a Refinement Region can give similar benefits with less overall mesh count.
If its possible, feel free to take a cutplane vertically through the model and show Velocity and have it Shaded Mesh and post it here so that we can see the mesh quality you have.
Overall the mesh doesnt look too bad around the device. The one aspect that I was mentioning in my previous comment is to add a refinement region above the device (vertically). As we are dealing with subtle density differences to generate the flow field and develop above the device, we will need a mesh to capture these details.
In the image below I've outlined where you would place your refinement region (in CFD) and refine the mesh a bit tighter.
Did you atempt trying Apolo's suggestions with the refinement region above the device?
Here is a nice discussion regarding refineing the mesh above the device in a natural convection application.
Some users prefer to the method discussed above and other will place a refinement region above the device without it actually overlapping the device to just refine the plume rising towards the outlet.
Dear Apolo and Royce,
Thanks for the support. Yes, it worked, but struck with another issue.
Some inputs from a new user: it was difficult for me to locate a specific surface/volume within th emodel to locate meshing error. I had a call with your support team to identify this.
your support team asked me to use Royce method. i am trying it and the results are promising. Thanks again for the support.