[ghorrocks]

mesh resolution near wall for laminar flow can be decided based on grid convergence studies.

Correct.

Can porous media be a major contributor to non-convergence?

Yes, definitely. In fact I know there is an update in V13 to improve the convergence of porous regions. This may fix your entire problem if you are not using the current version.

[Chander]

Originally Posted by ghorrocks

1c) I first of all determine whether a turbulence model is appropriate. In your case it is not. But if it is a turbulent flow then my default option is SST and I would only choose anything else if I had a specific reason to do so - eg anisotropic, bluff body etc. And yes, meshing is very important. The mesh is tailored to the boundary layer I expect to generate.

Originally Posted by ghorrocks

No it does not. If you use the k-e model in a laminar flow it will give you more dissipation then is really there, so is a significant source of error. The SST and related models are better here because they degenerate to (almost) laminar flow at low turbulence energies.

@ghorrocks

for the lowest inlet Re of 600, laminar transient model seems to be converging. I am now checking if my main variables of concern (pressure drop and maximum temperature in solid) have stabilised with respect to iteration count i.e. time. Then I can stop the simulation take the result as my evolved steady state solution. I am also trying to see if I can spot any oscillations in velocity pressure etc. by observing them at specific monitor points.

I am also doing the same transient run at higher Re of 1000. Here I am trying with both Laminar and SST model. As you said above , SST model is better than k-epsilon in low Re flow. However, today I came across a publication where the authors argue that even SST model should not be used for low Re and transitional flow. (http://ntrs.nasa.gov/archive/nasa/ca...2008023429.pdf)
In case I find that in my transient simulations, for higher inlet flow Re like 1000-4000, either the laminar model does not work or there is significant difference in results of the laminar and SST models, then do you recommend that I should try using SST model with the transitional model enabled in CFX? I spotted another thread where a model called the gamma-theta transition model has been recommended.( http://www.cfd-online.com/Forums/ans...lon-model.html )
I personally am sceptical about how good this transitional flow modeling is .

[Chander]

Originally Posted by ghorrocks

Correct.



Yes, definitely. In fact I know there is an update in V13 to improve the convergence of porous regions. This may fix your entire problem if you are not using the current version.

Oh Ok. Thanks for this important info!
Unfortunately, ver 13 is not available yet at the central cluster where I run my simulations. I'll have to make do with ver12.1 for the moment.

[ghorrocks]

The gamma-theta transitional model was developed for transition on airfoils. Your thing looks nothing like an airfoil so I do not think it will work very well for you.

I agree that the SST model should be avoided for transitional flows without the transition model. It is better to use a laminar model in a slightly turbulent flow - it means you are doing a pseudo-LES simulation but at very low Re the turbulence structures are large so this is OK; rather than use a turbulence model in a laminar flow.

Sounds like you need to lobby your cluster support people. If V13 simply fixes your problem then just imagine how much time you have wasted. And if your support is current you are entitled to this software so the only reason you don't have it is because IT have not installed it..... Multiply your hourly rate by the time wasted and you have a strong case to get it fixed ASAP. If you are a student, well the equation is a bit more tricky

[Chander]

Originally Posted by ghorrocks

It is better to use a laminar model in a slightly turbulent flow - it means you are doing a pseudo-LES simulation but at very low Re the turbulence structures are large so this is OK; rather than use a turbulence model in a laminar flow.

If you are a student, well the equation is a bit more tricky

Glen,
I did not get your comment regarding pseudo-LES simulation. Can you elucidate a bit on that?
Yes I am a PhD student
Actually our cluster people had tried to upgrade to ver 13 sometime back but they found some issues with parallalization with ver13. so they decided to stick to ver 12.1
ver 13 would have helped a lot as you said it has non-thermal equilibrium model for porous media also

One thing regarding porous media. I can simulate the pressure loss by modeling porous media simply as fluid domain also by only using the source term for momentum loss. I know this is not accurate as the effect of porosity is not accounted for in other terms of the Navier-Stokes equation. Have you tried with this approach? How good/bad it is in terms of accuracy and convergence?As far as the thermal part is concerned, if I stick to thermal equilibrium assumption, the fluid domain approach should also work. I am not sure though in case of non-thermal equilibrium.

[ghorrocks]

I did not get your comment regarding pseudo-LES simulation. Can you elucidate a bit on that?

If you are doing it right you will probably get some non-steady turbulent scale fluctuations starting up. This is effectively LES.

Actually our cluster people had tried to upgrade to ver 13 sometime back but they found some issues with parallalization with ver13. so they decided to stick to ver 12.1

My preferred approach would be to fix the problem. You have paid for the software, so install it and use it. Not installing it is just making things hard for yourself for no reason.

I can simulate the pressure loss by modeling porous media simply as fluid domain also by only using the source term for momentum loss.

Correct.

I know this is not accurate as the effect of porosity is not accounted for in other terms of the Navier-Stokes equation.

The porous model in CFX (to my knowledge) just applies a source term. So it is no different to applying the source term yourself. I do not expect it to be any more accurate.

[Chander]

Originally Posted by ghorrocks

The porous model in CFX (to my knowledge) just applies a source term. So it is no different to applying the source term yourself. I do not expect it to be any more accurate.

Actually the CFX manual mentions that the difference between full porous media model and fluid model with momentum loss terms is that in the former porosity affects all the terms of Navier-stokes equation and not only the source term as in the latter approach. It also states the modified equations for the full porous model.
I was thinking what difference will using a fluid model with momentum source term make in my simulations in terms of convergence and accuracy.
Regarding ver13, I`ll continue to try and get it

[ghorrocks]

I was not aware of the difference in porosity models. You learn something evey day.

If I was you I would trial the momenum source approach anyway. Maybe set up a simple benchmark simulation and compare if they are any different for flows similar to what you are looking at. If there is not difference then use whatever is easiest to get working properly.

[Chander]

Yes, I should probably try that.
Thanks again for your quick and patient replies

[Chander]

@ghorrocks

Hi Glen,
I am attaching here a cross-section of my mesh along with yplus plotted in that cross-section. Can you have a look at this and advise any changes if required?

Meanwhile transient simulations are showing promise. Thanks again for guiding in that direction.

[ghorrocks]

As I said in the other post you do not need to make porous domains different domains. You can make them sub-domains of the entire fluid domain. It probably won't make any difference but it is worth a try.

[Chander]

Yes, I will try that.
I just wanted to check with you about the nature of mesh (uniform) and the y+ at the wall . Is this kind of mesh and this much resolution good enough/ overkill or nit sufficient if I have to use k-omega based models for flow Re in the range of 1000-4000.

[ghorrocks]

You need to do a mesh refinement study to determine if your mesh is adequate. You cannot tell by simply looking at it.

Lots more detail is here:
http://www.cfd-online.com/Wiki/Ansys...publishable.3F

[Chander]

Ok.

Certainly, I will do a mesh refinement study.
I am familiar with GCI method and have used it before. You might recall , I had discussed that with you a few months back here