I am new to CFD Simulation.
I have an assembly, a nozzle head (with 4 inlet surfaces), and a filter section (outlet) and I am trying to simulate the airflow in the room to see the flow distribution.
I assigned Boundary Conditions (volumetric flow rate-fully developed) to the inlets, and a static gage pressure of 0 at the outlet.
I supressed he solid objects, meshed the air volume and ran the simulation.
I am getting incredibly high velocities (to the 6th power), and it looks like there is one small section (where the filter meets the nozzle head) that the high velocities are. Also, I solved it using flow and the default settings (ADV1) for 750 iterations.
I took a look at the Summary File, and I have:
Total Mass flow in: 4.26 lbm/s
Total Mass flow out: 1120.67 lbm/s
How can I fix this?
Solved! Go to Solution.
They red circles are the flow inlets, the gray cylinder is the outlet (at 0 psi gage static pressure), the 4 nozzles are radially symmetric (and the gray and blue cylinders as well). The setup is in the middle of the air volume.
The high velocities (usually 4-7 million in/s) occur at the location marked A (and this high velocity does not occur on the other side).
If this second shot helps, I am in the middle of running another sim with the same model, and its showing the velocity vectors. This is only iteration 250/750. But as you can see, the velocity distribution around the middle where the top and bottm parts meet is not uniform.
Thanks for your help, any insight is appreciated.
Are you modeling the walls as surface materials? If you PM me the model I can take a closer look, just send me a download link from dropbox or A360.
From a cursory observation, I think this is a case of divergence.
Have you tried reducing the factors in Solve Dialogue box >> Solution Control to 0.3 from 0.5?
Also I have seen divergences in very coarse and bad meshes. Make sure you have fine enough mesh to capture the flow physics and gradients.
I think you are right about divergence. Sometimes the solver quits and gives that error.
I have not yet tried your suggestion regarding the solution control.
Regarding the mesh, the mesh I used most recently is below (the spot where the high velocities occur is at the location where the top part meets the bottom part. No Interference from the CAD model, no gap between the parts, and the high velocity region is not radially symmetric, even though the model is).
Is that a bad mesh?
The problem has been resolved!
According to this forum post http://forums.autodesk.com/t5/Simulation-CFD/Perio
I wanted to get into more detail about this one, but ADV5 is a potential solution, but might not help in all cases here.
What you have going on here is a case where the 0 pressure boundary condition is very much within the flow domain. In general is a bad idea. The solver expects that the flow is fairly developed before it goes into the 0 pressure. This is why in the help we suggest to have inlet and outlet extension and really emphisize the outlet extension. The inlet extention is also a good idea so that a better mesh can be formed on the inlet face, the small duct helps better define mesh enhancement layers at the inlet face.
So, where does the air go when it goes through the 0 pressure boundary condition? Could the CAD be altered in such a way that we can duct that air out somehow?
ADV5 because of the tighter numerical methods will have the most potential to be stable in this sort of situation. Adjusting the solutions controls might have helped or more likely it will just delay the onset of the divergence.
Some extended thoughts. When solving with the k-e turbulence model you should limit your usage of mesh enhancement to between 3-5 layers. Using 10 layers is overkil, especially for this type of analysis. Keep the layer factor at 0.45.