"trapped" variables in rotating region

[marco.mueller]

Hi,

I often face the fact that velocity and pressure results are clearly dependent on the rotating region, like in this picture:

Even if I:

• have constant and small mesh sizes
• use ADV 5
• use small timestep size (3 degree rotation)
• solve hundreds of iterations

Is there any thing I'm missing here?

Thanks

Marco

[Royce_adsk]

Hi Marco,

What if you turn on ISC and run for a few hundred iterations?

What does the mesh look like on a cut-plane?

[marco.mueller]

I didnt try to use ISC.

[heath.houghton]

Have you tried smaller timesteps?  There have been some cases where you might need 1 degree per timestep depending on the rpm.

[marco.mueller]

I started with 90, then 9, finally 3. Did not try any further since it did not change between 9 & 3, also because its just 20 RPM and a high viscosity fluid (~ 5 Pas).

[Royce_adsk]

Try ISC and let us know how that works our for you.

-Royce

[srhusain · Accepted solution]

I might add that for high viscosity, the prescribed time step size will need further reduction- the advection scheme calculates a local (element based) characteristic time which can become very small due to large viscosity and the user prescribed time step has to be smaller than this for accurate time-stepping.

Often, using ISC will cause the solver to estimate a time step that satisfies the stability condition (CFL), but for high viscosity, due to above, even smaller time step size may be necessary.

So, if ISC does not mitigate the issue, you can leave it on, but try progressively smaller time steps until you get the expected qualitative behavior.

Hope this helps.

[marco.mueller]

Well, I thought a high viscosity would not require such a small time step.

Here are the results, though the magnitude changes, there is still a remarkable gradient at the edge of the RR:

200 x 0,75 s (90°):

+ 1000 x 0,075 s (9°):

+ 200 x 0,025 s (3°):

+ 2000 x ~0,01 s (ISC on, ~1°):

But anyway, looks as if this one was still not converged:

[marco.mueller]

So, finally I did a run with more iterations at the beginning, which solved the issue. To be honest, I dont know why I changed the time step size after just 200 iterations, which was way too early.

Thanks for your help!

[heath.houghton]

Can you post a picture of the good run?  It might help other users to see the difference. 

Thanks

[marco.mueller]

still not converged but getting better... 🙂

[Anonymous]

Hi Marco,

Could you please advise on the set-up that you used to solve this? 

I have a similar problem where by  I am trying to predict pressure loss through a measuring device (water) with a "rotor" in the middle. I have set the initial conditions of an inlet velocity of 400m3/hr and outlet pressure 1 bar. 

Did you have to apply any enhanced meshing to solve this? 

Which turbulence model and advection scheme do you use? (I am applying SST Omega and ADV5) 

Finally how did you work out the time step size and no. of time steps? (the "rotor" in my case has an RPM of around 2225). 

I will also appreciate if someone from Autodesk support can shed any light on this problem. 

PS: Please go easy this is my first post and I am new to CFD 🙂 

Thanks,

Paren 

[Jon.Wilde]

Not wanting to hijack this case as Marco is doing a great job but check out the guide here. The Courant-Freidrich-Lewy (CFL) number ought to help you decide on a sensible time step 🙂

[Anonymous]

Hi John,

Thanks for your reply. I have just seen your reply on my other post too. That will keep me busy for the weekend! 

Regards,

Paren