[svantevid]

Hi!

I'm setting up a simulation of a centrifugal air pump with multiple reference frame model (1 rotational domain with the pump geometry and inlet space, 1 stationary domain with the pump outlet). steady, k-eps turb model, enhanced wall treatment, mesh is well inside the recommended metrics, pressure based solver, coupled scheme, massflow outlet, pressure inlet.
I was following the Ansys tutorial we received at the Ansys training class and I noticed that the simulation is run with a small (0.1) time scale factor.

When I was preparing my simulation, I could not get it to converge with a time scale factor larger than 0.5, actually the best strategy was to run it at 0.1 for a few 100 iterations and then a few 1000 with 0.5. Whenever I changed it to 1, the case diverged and threw a floating point error. The divergence starts with the epsilon residual and the velocities at the outlet go through the roof.

But the main problem is that the massflow rate at the outlet does not match the prescribed on, it's always larger. When I switch the time scale factor to 1 it starts to get closer to it, but then always the case diverges.

I'm fairly new to CFD and I cannot wrap my head around the time scale factor concept.

[NickFL]

The time scale factor is basically used as a speed limit on the convergence. It is analogous to the relaxation factors of the SIMPLE method. Basically, we are using an iterative solver and the factor is used to say how much we can change per iteration. A higher value means the solution can change more per timestep. While that might sound good, it also has some drawbacks.



Think back to another iterative solver in Netwon's root finding method. Here if you chose a bad starting point the derivate could send you far away from the root that you are trying to find. By putting in a factor that limits how far the solution changes per iteration. This is exactly analogous to what you are finding with your solution. At the early iterations you use a smaller timescale factor to prevent it from being sent off to infinity. Once you are “closer” to the solution, you can use a bigger timescale factor to push you to the solution faster. That is what you have done by increasing the timescale to 0.5.



Now your problem is still much more complex than Newton’s method. You have a rotating domain, you have boundary conditions, coupled equations, etc. And what time step Fluent “chooses” for the pseudo time integration is basically a proprietary black box. If Fluent suggests that it should be 0.5 for such problems, it already knows that the “guessed” value is a little aggressive for this type of problem. The important thing is it does not matter. The solution will converge to the solution for the geometry/grid/boundary conditions/etc. independent of this factor. It will just take a few more iterations, giving us more time to drink coffee. If it doesn’t converge, we swear at Fluent for making a bad choice, adjust the timescale factor (or give a better initial condition) and try again.


Now with all that said, I am concerned about mass flow condition. The solver isn’t matching what you put in as a boundary condition? Is there any backflow at the outlet? Do you have this as a monitor point during the solution? How does it look as the solve progresses?

[svantevid]

Thanks for the explanation, everything makes much more sense now.

Regarding the outlet; no, there is no backflow. I am monitoring the mass flow rate at the outlet, the calculation always starts with a slightly higher (5-10%) massflow rate than the BC I defined, then mostly always drops and at some point rises and stays aroung 20-30% larger than BC before it suddenly starts rising rapidly.

[NickFL]

How does the mass balance look (difference between inlet & outlet)? What interface model are you using? How are the residuals behaving?

[svantevid]

After I made another round of detailed checks of all different flow parameters, I noticed the flow at the outlet was, for the lack of better words, slightly odd. I then reduced the size of the outlet area (volume between pump outlet and actual domain outlet).

This somehow solved the problem; there is no more divergence and the difference between set and actual mass flow are at the outlet is now less than 1%.