[mosquera]

Hi everyone,

I've been working on a case for several weeks and have been having serious convergence issues with simpleFoam.

I'm using a realizable k-epsilon model and attempting to model channel flow. Initially I have been doing a 2d simluation in order to verify the flow at a later point downstream. I have experimental hotwire data and have calculated k and epsilon to be applied as a boundary condition at the inlet of the flow. From here I hope to have the flow develop and compare it to experimental data further downstream for model validation.

I've initialized with first order schemes but have been unable to move to second order schemes.

The link to the dropbox folder is https://www.dropbox.com/sh/uwz01qxgllmsval/4XGWNlb2V2

The relevant files are under CFDOnlineHelp. The case is under helpme with the excel file used to calculate k and epsilon under the same folder. The k and epsilon applied at the boundary are from columns j-q, with q being the k applied.

Unfortunately time constraints have become an issue, so I am somewhat desperate for any assistance.

Any guidance or assistance would be tremendously appreciated,
Matt

[gillimaniac]

Hey,

first thing i recognized while looking through your (non-common) case files is that you are using LowRe formulations in your boundary files (e.g. epsilonLowReWF, kLowReWF and nutLowReWF). Modeling the viscous sub layer (e.g. LowRe simulation) would need an y+-value of <=1. According to your attached yPlus.gz your mesh provides only an y+ of 33,5 which would be sufficient for high-Re simulation but not for LowRe.
This would be a starting point to look at i think.

[mosquera]

Hi Stefan,

I actually made some serious progress yesterday (which is typical. You ask for help and figure it out twenty minutes later.) What ended up being the issue was that the mesh was nondimensionalized while the velocity, k, and epsilon had associated dimensions. I scaled the mesh and things are going much more smoothly now.

Do you know offhand if having a y+ significantly less than 1 would pose any issues? I understand it's computationally expensive but other than that are there any issues?

Cheers,
Matt

[gillimaniac]

Hey Matt,

Y+ < 1 shouldn't bring you big issues as long as you resolve the complete boundary layer region with your inflating boundary layer mesh.
Figure 3 on the following site shows what I mean: http://www.computationalfluiddynamic...oundary-layer/
Significantly lower Y+ values than 1 are simply unneccesary but shouldn't be a problem i guess. But im also still in the learning process regarding simulations' Y+ behaviour

[mosquera]

That's great to hear.

Once I dimensionalized my simulation the convergence improved greatly. I'm actually running the three dimensional cases now.

I'm still confused about residuals. FOAM defaults to converging around 1e-05 for residuals, but it seems as though that's more of a guideline then anything else. Is it possible that I could have convergence with a higher pressure residual because of the nature of my inlet BC?

Thanks,
Matt

[mosquera]

Specifically I'm looking at the k and epsilon residuals. Whoever worked on this previously said that convergence took place when the k and epsilon values had residuals of 1e-03. Is this valid?

Thanks,
Matt

[gillimaniac]

I've read this a couple of times too. It sais so, because changes below 1e-3 are not recognizeable by eye anymore.
But personally i'd like to get the initial residuals at least below 1e-5.

Additionally in complex cases I always look at the values of probes distributed all over the domain.

cheers

[mosquera]

I managed to solve that convergence issue, now I think my troubles are down to properly specifying k and epsilon at the inlet.

I've been using the following site to calculate the turbulent kinetic energy and epsilon based on the fluctuating velocity components;
http://jullio.pe.kr/fluent6.1/help/html/ug/node178.htm

Is that turbulent length scale l valid for calculating epsilon? What's the difference between a turbulent length scale and a turbulent mixing length? I can't seem to find anything differentiating the two.

Thanks,
Matt

[gillimaniac]

Hey good to hear that you are getting further.

The difference between a turbulent length scale is not too easy for me to explain but on the site you quoted (which i also am looking at some times) it says:

l = 0,07 L

where L is a physical length of the domain. Most times this refers to the hydraulic diameter which corresponds to the diameter in case of a circular pipe.

l is the so called turbulent length scale which you can use to estimate the values of k, epsilon, omega or the eddy viscosity.

The factor 0,07 in this formula is based on the maximum value of the mixing length in fully developed pipe flow.

This describes briefly how the mixing length and the turbulent length scale can be calculated by each other.

If you want to know more about the mixing length theory i think you will have to look deeper in some papers discussing this thematic. But what is always true for both lengths is that they will always be smaller than the geometric length (eddy diameters will never be bigger than your pipe diameter for example).

This is little scientific and perhaps also little help for you but before monday i wont have time to dig in deeper into that topic.
Others around here can surely tell you more about this topic.