Discussion Forum

Hi,

I would rather have a look at the dimensionless wall distance and at the dimensional wall distance. It may be of interest also to plot the ratio of the turbulent viscosity on the dynamic viscosity, usually the ratio is over 100:1.

It is hard to gauge the variations in K and epsilon from the images but it seems they are fairly small oscillations.

Cheers

Hi Amir,

thanks for replying. I am sorry for asking this, but how do I plot the dimensionless wall distance and at the dimensional wall distance? Neither of these variables appear in the plot menu...

If you could give some hints I would appreciate it.

Cheers.

Rui

Hi,

In any surface plot you select 'Turbulent flow' and then in the list there are 'Wall lift-off (mod1.spf.delta_w)' and 'Wall lift-off in viscous units (mod1.spf.d_w_plus)'.


Cheers

Hello Amir,

here are the screenshots. And thanks for the tips.

I'll be looking forward for your assessment.

Cheers!

Hi,

I think that first of all you may want to study about what boundary layers are, the best introductory book I have found so far on boundary layer theory is 'Foundations of boundary layer theory for momentum, heat and mass transfer', J. Schetz, ISBN 0133293343.

For this time a very brief summary may be in order. Turbulent flow is characterized by very large variations in the velocity field; comsol uses a mathematical technique to approximate such variations, known as Reynolds average, so that it computes for the mean velocity components. A major characteristic is that it does not solve for the fluid motion at the wall and very close to it, such region is known as a boundary layer wherein velocity grows from zero (at the wall) to some value close to the average velocity of the bulk of the fluid. In this case the boundary layer is said to be turbulent and can be divided into three sub-layers, laminar, intermediate and turbulent ones (or similar names). Because comsol does not solve for any of these three sub-layers, it is crucial to make sure that its approximation is sound enough, to wit, that the dimensionless distance from the wall is 11.06 or very close to it, and at the same time that the dimensional distance from the wall is very small compared to some characteristic length.
I know this is an extremely short version of it all but I would strongly suggest to study the theory first of all. Even in the comsol manual there is something to chew on.

In this case the dimensionless distance hovers a bit above 11.06 which is not bad but it oscillates maybe a bit too much. The dimensional distance ranges from less than 1mm to more than 1mm, it sounds suspiscious. However, the images are not easy to read. It is also important to relate the dimensional distance to the characteristic legth of the problem, which I would say is the diameter of the pipe.

How to correct for problems with the d_wall and w_wall_plus? By intervening on the mesh close to the boundary of the geometry, that is by making the first boundary layer much closer to the wall (maybe the distance from the boundary for the first one should be less than 1mm) and use quite a number of boundary layers (5, 6, 8, 12?).


Cheers

The k-e model attempts to resolve the viscouys sublayer and in order to do this satisfactorily, the mesh must be fine enough to have a dimensionless wall distance (w_wall_plus) of less than 5. Why does Comsol specify 11.06 for the w_wall_plus? Its a bit worrying for me as this is an order of magnitude more than the literature specifies. I know other CFD packages like Fluent are in agreement with literature but cannot explain why Comsol gives a different value for the wall lift-off?

Can someone please shed light on the matter

Appreciated.

Hi,

First of all you may want to read the manual, page 168 of the CFDModuleUserGuide and following, it explains why they chose 11.06; to put it very briefly they decided to consider some half-way point between the viscous sub-layer and the logarithmic layer. The k-epsilon model does not solve for the viscous sub-layer, somehow it can be tweaked to do so or approximately so, again you may want to read the manual.

Specifically regarding the decision to let the sub-layers meet at half-way, there is some room to debate the correctness of such an approach. However from the practical point of view you'd better to keep under control the dimensional lift-off distance, i.e. it must be much smaller than dimensions of your fluid domain.

Cheers

Hi Amir. Thanks for the insight. Do you have the manual at least the part that has turbulent flow modelling. I have been getting bits and pieces of the v4.2a manual on the internet but never the whole manual. Also i cannot explain the overshoot that one gets for the velocity profile at the centreline/axis particularly in the developing region when considering pipe flow (see attached png).

Hi,

I think the manual comes with the installation DVD, or you can simply ask for a copy to your local Comsol representative.

The overshoot seems to be just a numerical artifact, something similar to a Gibbs phenomenon. It may be related to your mesh (try decreasing the size of the elements) or you may use artificial diffusion to get rid of it, making sure you do not alter the 'physical acceptability' of the solution.

Cheers

Thanks Amir, I have just checked with the installation guys, we dont have a CFD module so that user guide manual i cant have it. I tried second-order elements and the overshoot disappeared, thanks for that. But you also talked of artificial diffusion as the other way, what is that and how can it be effected. Also, i have been doing pipe flow simulations in a smooth pipe, how do i present a rough surface in Comsol?

Cheers.

Hi,

Artificial diffusion is just another name for inconsistent stabilization techniques, you may find it under the 'Stabilization' -> 'Inconsistent Stabilization' tag under the Turbulent Flow node.

As the name says it causes the solver to find an inconsistent solution, i.e. a non physical one, by smoothing out eventual spikes. It can be useful to get rid of Gibbs phenomena or similar issues, if re-meshing or different order shape functions are not enough.

I have tried a bit but then given up on rough surfaces in Comsol especially for turbulent flows. They may be implemented with laminar flows, but I strongly doubt they could ever be implemented with turbulence in Comsol.

Cheers

I am thinking that perhaps since the first computational cell is off-wall, then it would not really matter whether you are considering a smooth surface or not. And how did you do it for laminar flow?

Hi,

Practically, surface roughness may destroy the laminar sub-layer of the turbulent boundary layer, thus it may affect turbulent flows greatly. Furthermore, Comsol approximates the solution by using wall functions starting at an imaginary intersection between the laminar and intermediate sub-layers, how close to the physics of the problem is such an approximation when surface rougness is involved? Who knows!

I did not 'do it for laminar flows', I started with some ideas but I am not interested in laminar flows; you may start by simply adding some drag force on the surface.

Cheers

Thanks let me try will revert in due course. And thanks for the insight.

Cheers

Hi Amir,

The new pipe flow module makes it easier for us to incorporate surface roughness in fluid flow in pipes. With this module, you can specify the surface roughness as well as your friction model (Haaland, Colebrook, etc). Interesting.

Cheers.

Hi,

Pipe flow module can be applied if and only if you have pipes long enough so that entrance length has no or little influence over the velocity profile. It is an interesting one dimensional simulation tool but with a very limited applicability.

I already tested it for large plants, it seems to provide reasonable results. It is useless to model specific devices. It all depends on the goal of your simulation.

Cheers

Hi,

Yes i see where you are coming from, in my case i was trying to see the effect of surface roughness in a model i had initially done assuming smooth surface. Mainly to see the effect on presure drop over the range of velocities that i have been using. I also see you do not get much information besides the pressure differential. And i agree with you it may all look useless.

Cheers.