[Chris_321]

I did a basic simulation around these twisted cylinder profiles at Re ~ 400



The problem im facing right now is, that i can't reach a proper convergence in transient simulation.



The v and w velocities are already like expected, but the u velocity looks a bit strange. I expected some uniform sine waves( Karmann street) like v and w velocities, but it looks more like a non periodic signal.


I use adaptive timestepsize with a target of a max courant number of 10.
Is my timestep size to large( the courant number to high?)? I dont think it is an issure of the mesh, because i already did some basic sensitive studies.

Should i use some under relaxation parameters?

Or is it just the physics and the flow will change with a spektrum and not with just one frequency? At a previous "flow around a cylinder" 2D simulation, i could determine a single frequency which match a calculation by hand with the strouhal zahl.

[ghorrocks]

I use adaptive timestepsize with a target of a max courant number of 10.

A better approach is to use adaptive time steps homing in on 3-5 coeff loops per iteration.

Should i use some under relaxation parameters?

No

Or is it just the physics and the flow will change with a spektrum and not with just one frequency?

That is possible. Have a look at the transient results file and see what the flow feature at the different frequency is. Then you might have an idea of whether it is likely to be real or not.

[monkey1]

As for your problem with the axial fan...I would have also a look to the time elapsed. You simulated "only" 0.04s of time. Is this sufficient for the flow to become fully developped and "constant" when starting from an initialisation?

[Chris_321]

Thanks glenn, i will give the number of coefficient loops option a try.

In the Solver control i have the min and max coefficent loops and in the analysis type setting i have the target min max coefficent loop. What is the difference?


@monkey
I initialized with a Kelvin-helmholz instability.
The flow becomes "steady" after 0.03 s


If i use a smaller timestep ( static size that is changed by hand to 50% of the average timestep size that the solver used with the adaptive settings) then the change in the u- velocity value looks mutch better.

[ghorrocks]

If i use a smaller timestep .... then the change in the u- velocity value looks mutch better.

Then your time step size is way too big. Either do a time step sensitivity study to determine what is required or let the solver find it with adaptive time stepping to 3-5 coeff loops per iteration.

Max and min coeff loops are just what they say - Min coeff loops is the minimum it will do, even if the convergence criteria is achieved. Max coeff loops is the max it will do even if convergence is not achieved. The max and min target are what it will adjust the time step size to achieve.

You normally set min coeff loops =1, max = 10, min target = 2 or 3, max target = 4 or 5.

[ghorrocks]

If i use a smaller timestep .... then the change in the u- velocity value looks mutch better.

Then your time step size is way too big. Either do a time step sensitivity study to determine what is required or let the solver find it with adaptive time stepping to 3-5 coeff loops per iteration.

Max and min coeff loops are just what they say - Min coeff loops is the minimum it will do, even if the convergence criteria is achieved. Max coeff loops is the max it will do even if convergence is not achieved. The max and min target are what it will adjust the time step size to achieve.

You normally set min coeff loops =1, max = 10, min target = 2 or 3, max target = 4 or 5.

[Chris_321]

The number of coefficent loops option makes me even more confused...

If i change to this method the u velocity becomes almost stable. The magnitude of the change is way smaller, than with the max courant number approach.



The timestep size used from the adaptive method is way larger than the size used by the courant approach




My residuals are higher aswell but atleast they became stable



How can i determine wich result is more accurate?
The max courant number from the number of coeff loops is about 30. ( Which makes sense if i think about the timestep size)
How should i go on? Lowering the timestep? Is it better to use a courant or the coeff loops approach and why?

[ghorrocks]

CFX is an implicit solver. Therefore Courant number is not a defining parameter in convergence - that is the reason I do not recommend it. The coeff loops approach makes the solver run at an efficient number of coeff loops automatically and it is rare for it not end up with an inappropriate time step size.

I would trust the coeff loops approach. This suggests your courant number time steps were too small and you were getting numerical round off problems which caused instability.

If you want to be sure, run a sweep of fixed time step size simulations from very large to very small. Compare the results on parameters of interest to you (maybe pressure loss of whatever) and I bet it initially converges, but after a while diverges as the time step gets too small.