[sidharath]

Hi all,
I am modelling the near surge point of a centrifugal compressor with DES in CFX 15.
I've attached the images of blending function and strain rate invariant.

I am seeking some direction on couple of points mentioned below:
1. As the CFX modelling guide says "In regions where the function is zero, the LES model is used, and the region where its value is one, the RANS model is activated". I can't see any 0 in my model, the lowest is of the order of 10^-2 but not 0.
Can anyone share their knowledge if 0 means absolute 0 in this case or a small value? Also, what about the grey region between 0 & 1. Is there any transition function involved or the grey region is to be avoided using grid / timestep refinement?

2. In the case of strain rate invariant, I can see only one scale. The theory guide suggests using reduced timestep, refine grid, use Fsst = F1 or Fsst = 0. I did try reduced TS and grid size but didn't see any more scales in invariant isosurface and don't really understand the Fsst = F1 / 0.
Can someone please share some pointers to what am I doing wrong and how can I navigate through this problem.

3. Acoustic courant number is always 999.99, any ideas why? Please correct me if I am wrong, CFX isn't highly dependent on courant number to accurately resolve unsteadiness and I can get away without maintaining the courant number as unity?? In this case, the RMS courant number is 19 and max are 952. Any inputs on this would be great.

4. I am currently using the 4-degree rotation of wheel per timestep as physical TS value and using 8 coefficients loops. I've seen the various post by Glenn and Ansys resources emphasising 3-5 loops to achieve the convergence in each TS by using necessary TS. I did use the lowest TS I could use to (computation power constraint) but still couldn't achieve the convergence in fewer loops. Any direction in here on what should be done would be incredibly useful. I have attached the plots of residuals too.

5. The objective is to model the in-duct pressure fluctuations leading to acoustic spectrum. Any do's and don't from this perspective are highly welcomed.

Thank you for contributing.

[ghorrocks]

I will answer your questions which I think I might be able to help with:

3) Then run a smaller time step and see if it makes a difference. It is best to establish these things yourself using your simulation.

4) 4 degrees per time step sounds very large, especially for a DES/LES model. Are you using double precision numerics?

Also you will need to check your mesh is OK. Have you done a mesh sensitivity check?

[sidharath]

Thank you for the inputs and reply, Glenn.
3. I am planning to do a time step independence study but the computational constraints are in the process of sorting out.

4. 4 deg is large but there is published literature with similar timestep size. I am running one model with 2 deg TS too but results aren't substantially different; RMS courant number drops to 12 but acoustic courant number is still 999.99
- Yes, I am using double numerics.
- I've done the mesh sensitivity/independence study but it's based on RANS rather than DES (i've attached the mesh study screen shot with the highlighted mesh as the one used in this model). I am not sure if it's the best way to go about it but computational constraints are forcing my hand this way. Although the cfx modelling guide does say that "While the grid resolution requirements are not significantly higher than RANS for simulations, the time resolution imposes high CPU demands."

Based on what I've read from your post, you prefer to use adaptative TS based on courant number target, you think I should try that approach instead even CFX isn't highly courant number dependent?

Thank you

[ghorrocks]

Mesh and time step sensitivity of DES/LES will be very different to RANS. You will have to redo it for a DES/LES simulation.

No, I recommend adaptive time steps homing in on 3-5 coeff loops per iteration.

[sidharath]

Originally Posted by ghorrocks

Mesh and time step sensitivity of DES/LES will be very different to RANS. You will have to redo it for a DES/LES simulation.

No, I recommend adaptive time steps homing in on 3-5 coeff loops per iteration.

Thank you for the recommendation.
I've set-up simulation with adaptive timestep and target of 3-5 coefficient loops instead of courant number and also dropped the convergence target for residual RMS from 10^-6 to 10^-4.

I don't think it'll possible for me with current resources to do a grid independence study for DES. It would be great if I can do a timestep independence study alone.

I'll update you how it goes and thank you again. I appreciate your time.

[ghorrocks]

I don't think it'll possible for me with current resources to do a grid independence study for DES.

Then how will you know if you have sufficient computing power to perform this type of simulation? If you do not have adequate computing power then it is better to know it cannot be done and not waste your time on a simulation which will not achieve your aim.

[sidharath]

Originally Posted by ghorrocks

Then how will you know if you have sufficient computing power to perform this type of simulation? If you do not have adequate computing power then it is better to know it cannot be done and not waste your time on a simulation which will not achieve your aim.

The grid independence study with add extra 6-8 simulations. It takes months to run one. Literature does suggest that performance can be predicted fairly easy with the mesh I am currently using.
I'll measure the acoustic PSD and correlate it with numerical results. I'll only work in the zone of similar trends between two and reason the computational constraints for not working on other regions.
Moreover, if i can see positive design effects using the current set-up, I can test to see the actual improvements and that should be enough for thesis ( I hope).

[ghorrocks]

You don't have to do the grid independence study on the full thing. Either cut out a section of the geometry or use a simpler analogy.

If it takes months to run then it is even more important to do all the checks in advance or you will be wasting months of time!

[sidharath]

Originally Posted by ghorrocks

You don't have to do the grid independence study on the full thing. Either cut out a section of the geometry or use a simpler analogy.

If it takes months to run then it is even more important to do all the checks in advance or you will be wasting months of time!

Hi Glenn,
1. I ran the adaptive timesteps with target min and max coefficient loops as 3 & 5 respectively. I specified the timestep range from 5 degrees /TS to 0.5 deg/TS.
Cfx ran till the least timestep value i.e. 0.5 deg/TS and still wasn't able to achieve the target residuals of 10^-4 and hence, was running with 8 coefficient loops (max specified in solver control). I've attached the relevant screenshots.
I don't think it'll be wise to reduce timestep any further, the computational requirements are already huge. I was wondering in your experience what would be the consequences of not following 10^-4 residual levels to the dot? This being said I've come across one paper which specified the residual targets as 10^-3 for near surge points. It's peculiar that not many research groups talk about the convergence criterion used by them in their papers and validates directly with test results.

2. Would cut out section is credible for grid independence study? As in, if I only model impeller section and leave out rest, although I do think immediate inlet and diffuser + volute sees a lot of (dynamic) instability (from steady state results and published work). You think if this will be a valid approach? and also, if you could elucidate on analogy, I am not sure what you meant by using analogy for grid independence.

Thank you.

[ghorrocks]

I don't think it'll be wise to reduce timestep any further, the computational requirements are already huge.

If it needs to go smaller then you have to let it. Also remove your artificial restriction of a minimum timestep of 0.5 degrees and let it go as small as it needs. DES/LES models require very small timesteps, that's how they work.

Would cut out section is credible for grid independence study?

As long as you can generate something which will have equivalent physics and length scales. I would think the tightest mesh size requirement will be the impeller and very close downstream. So just do this bit for the mesh study and remove the upstream and downstream runner.

[sidharath]

Originally Posted by ghorrocks

If it needs to go smaller then you have to let it. Also remove your artificial restriction of a minimum timestep of 0.5 degrees and let it go as small as it needs. DES/LES models require very small timesteps, that's how they work.

I extended the adaptive time step study and relaxed the minimum time step limit. To get the initial results, I ran the simulation with frozen (MRF) rotor interface rather than sliding mesh (transient rotor-stator). The residual target to 10^-4 rms is achieved with 0.095 degrees/timestep giving rms courant number of 0.56.
I'll run with this timestep and compare its acoustic psd with that of bigger time steps. This, in turn, should reinforce time step independence too.


As long as you can generate something which will have equivalent physics and length scales. I would think the tightest mesh size requirement will be the impeller and very close downstream. So just do this bit for the mesh study and remove the upstream and downstream runner.

I will work on these line and try to device some less computationally expensive form of mesh independence case.

One more thing, I was wondering if you've any directions for implementing anechoic termination/non-reflecting bc in cfx in order to curb the spurious reflections.
Thank you.

[sidharath]

It was in quotes in last reply, my bad.


I extended the adaptive time step study and relaxed the minimum time step limit. To get the initial results, I ran the simulation with frozen (MRF) rotor interface rather than sliding mesh (transient rotor-stator). The residual target to 10^-4 rms is achieved with 0.095 degrees/timestep giving rms courant number of 0.56.
I'll run with this timestep and compare its acoustic psd with that of bigger time steps. This, in turn, should reinforce time step independence too.

[ghorrocks]

Non-reflecting BC: A simple way of doing this which does not always work is to deliberately grossly coarsen your mesh immediately at the boundary. The wave hits the coarse mesh and gets dissipated by the coarse mesh. Use a GGI interface to connect the very coarse mesh to the finer main mesh. This method is crude but sometimes can work.

There is also a beta feature for non-reflective boundary conditions. Enable beta features in CFX-Pre and give it a try as well.

[sidharath]

Hi Glenn, thank you for the information and tips to employ nrbc.

I explored the beta options in cfx but as far as I gather, nrbc can be only employed at the inlet and not on the outlet. Is that so and if yes, what you think is the intent of it?

I've come across another method using "beamforming" (published by researchers in CMT Valencia) to resolve the reflection issue. I am reading and try to employ beamforming but haven't had any luck at this point in time. Would you have any idea about beamforming?
Thank you

[ghorrocks]

I have never used the non-reflecting BC in CFX. It is a beta feature anyway so it is not fully supported or documented. So I can't help you there.

I can't help you with beamforming either. If you want to go that way you will have to work it out for yourself.

Don't forget my suggestion of the grossly coarse mesh at the boundary - it is simple to do and has given quite good results for several people. It is so simple that surely it is worth a try.

[sidharath]

Thanks a lot for all your replies Glenn, I really appreciate your time. I should put you as my co-supervisor

I'll surely try the coarse mesh at boundaries and keep you posted about the success of methods and try to validate it with beamforming and experimental results as and when they work out.

Thank you once again.

[Tingyun YIN]

Hi, Sidharath and Glenn Horrocks,

Currently, I am working on the DES simulation. But I have some problems about the numerical scheme and want to ask for help.

When we switch on DES or SAS model in CFX, an additional option occur in the solver control plane. It's called 'CDS blending'. As is well know, different numerical schemes could be applied to different regions when using DES or SAS model: CDS for LES region and Second order for RANS region. So, here are my questions:

1. When we switch on the default DES model in CFX, the default numerical scheme is hybrid scheme? The advection scheme option is available only for RANS region because CDS is used for LES region as default. So, when 'CDS blending' is activated, there are two functions: The first one is to prevent the grid-induced separation (as default, minimum RANS blend= BF1=0, maximum RANS blend= BF2=1) and avoid oscillations due to the central difference scheme (as default, Maximum Courant Number=5, Limiter Exponent=1).

2. If the description of question 1 is correct, so, when we switch on the default SAS model and activate 'CDS blending' function, why minimum RANS blend and maximum RANS blend still occur? As we all know, no grid-induced separation occurs when using SAS model. So, what should I do? Don't activate them? To avoid oscillations of CDS, Maximum Courant Number=5, Limiter Exponent=1 can be activated.

3. If the description of question 1 is wrong, so, when we switch on the default DES model, we have to activate the 'CDS blending' to activate the hybrid scheme?

Any comments are appreciated. Thanks in advance.

[ghorrocks]

I do not know the answers to your questions so cannot help. All I can suggest is to read the documentation carefully and if you can't work it try ANSYS training and support.

[Tingyun YIN]

Originally Posted by ghorrocks

I do not know the answers to your questions so cannot help. All I can suggest is to read the documentation carefully and if you can't work it try ANSYS training and support.

Hi Glenn,

Fine. After checking Help Document, I still do not get the answers. That's the reason why I post questions here. Anyway, I will try ANSYS training and support later.

Thank you very much!