[Mason liu]

Hi, all,

this should be a basic problem, but really confuse me now. I have go through the related info with CFD wiki, but still have something I can't understand.

My case is simple: calculate the 2D drag coefficient of a profile(take one layer mesh in CFX to simu 2D), profile is a rounded corner trapezoidRounded Corners Trapezoid Profile.png.

Now I'm mainly doing steady state simulation, from all information like CFD wiki, all said that with a smaller timescale in SS simulation will help the convergence. But I found that's not in my cases. Please review below pic.
CFD-Online2015-12-08Q.png

That's picked 5 cases with different timescale(auto timescale-conservative / auto timescale-aggressive / physical timescale =0.001s / 0.01s / 0.02s), I have checked the timescale in output file, auto timescale-conservative =0.0038s , auto timescale-aggressive =0.036s, so my timescale range is[0.001s, 0.0038s, 0.01s, 0.02s, 0.036s].

From above pic you can find that:

1. With smaller timescales(0.001 / 0.0038 0.01) the convergence is very bad, Cd and Cl curves varies lot and residuals not good, too.
2. But with some bigger timescales(0.02 / 0.036) the Cd curves is steady with tiny fluctuation, althrough residuals not good enough, but some better.

Anyone please give some advice on this? This doesn't make sense!

And, what about my residuals level? Is that two still too high? they can't go down with current mesh and setting, so if this is a problem then I'll start to correct this.

thanks really.

[Mason liu]

Anyone please...
I'm using SST turbulence model and max Y+ is below 1, about 0.3. Re around 9e5~1e6.

[ghorrocks]

This is discussed in the FAQ: http://www.cfd-online.com/Wiki/Ansys...gence_criteria

You will find that many bluff body flows are transient, so this is a very common problem. So you may need to run this as a transient model.

[Mason liu]

Originally Posted by ghorrocks

This is discussed in the FAQ: http://www.cfd-online.com/Wiki/Ansys...gence_criteria

You will find that many bluff body flows are transient, so this is a very common problem. So you may need to run this as a transient model.

Thanks ghorrocks really.

I have reviewed the FAQ, FAQ mentioned that if important monitor point can't converged, then can try "Use a larger physical time step", now from my cases(listed in picture before) seems that this will make monitor point converged, but I think that residuals still are not converged enough.

ghorrocks, do you think my cases(physical timescale=0.02 and aggressive timescale) converged?


And I also run several steady state and transient cases with same model, Angles.jpg. you can find in pictures. There are 5 models with different angles.

Now my transient cases told me that : Cd is 5<0<10<-5<-10, but steady cases give me Cd is -5<-10<0<5<10.

This really make me confused, and the transient cases show unsteady flow, vertex shedding is there#55 vorticity z.jpg.just in this picture.

Could you please help to give some advice on this, now I don't know what need to do, thanks a lot.

[ghorrocks]

Bluff bodies like this frequently shed transient vorticies. As this is a major part of your simulation I would not be happy running that steady state. You will need to run this transient.

[Mason liu]

Originally Posted by ghorrocks

Bluff bodies like this frequently shed transient vorticies. As this is a major part of your simulation I would not be happy running that steady state. You will need to run this transient.

Thanks ghorrocks.

That means that steady state simulation is not right? O, I used to run steady cases before.

Now my two transient cases(with different advection scheme and solving order) show different Cd and flow pattern, if two are all converged, then with higher order scheme should be more accurate, right?
Thanks a lot for your help.

[ghorrocks]

The test is quite simple: Compare a steady state run to a time-averaged result from a transient run. If they are the same within a tolerance you are happy with then the SS run is fine. But in my experience you cannot model significant vortex shedding with a steady state simulation, it results in quite a large error.

Don't take my word for it, it is a simple check to do for yourself.

Yes, the higher order scheme should be more accurate. But a result like this suggests you are still in the mesh sensitive region which means neither of the runs is likely to be accurate. You will need to run a mesh sensitivity check as well.

[Mason liu]

Originally Posted by ghorrocks

The test is quite simple: Compare a steady state run to a time-averaged result from a transient run. If they are the same within a tolerance you are happy with then the SS run is fine. But in my experience you cannot model significant vortex shedding with a steady state simulation, it results in quite a large error.

Don't take my word for it, it is a simple check to do for yourself.

Yes, the higher order scheme should be more accurate. But a result like this suggests you are still in the mesh sensitive region which means neither of the runs is likely to be accurate. You will need to run a mesh sensitivity check as well.

Thanks Ghorrocks.

Yes, you are right, the SS results and averaged results from transient are not same within a certain tolerance.

So I want to refine the mesh in wake region. Don't know if this'll matters.

Thanks Ghorrocks really. I'll let you know the results.