CFD Online Logo CFD Online URL
Home > Forums > General Forums > Main CFD Forum

length scales at inlet for internal flows

Register Blogs Members List Search Today's Posts Mark Forums Read

LinkBack Thread Tools Search this Thread Display Modes
Old   July 2, 1999, 08:18
Default length scales at inlet for internal flows
Anne-Marie Giroux
Posts: n/a
I compute flows in hydraulic turbine components with TASCflow (which uses the standard k-e turbulence modelling) and I don't have a systematic way to define the length scale (or dissipation rate of turbulent kinetic energy) as a boundary condition for turbulence at inlet. Can someone help me ? (Any reference on that subject would be appreciated)
  Reply With Quote

Old   July 2, 1999, 13:48
Default Re: length scales at inlet for internal flows
John C. Chien
Posts: n/a
(1). This is a very good question. It is also an important one which will remain so for a while. (2).The two-equation k-epsilon model was developed for boundary layer flows. So, inside the boundary layer, there are data available for velocity, turbulence kinetic energy, shear stresses, length scales, dissipation of TKE, and eddy viscosity, etc...... (3). In the two-equation k-epsilon model, the eddy viscosity is expressed as a function of k and epsilon. (and some known coefficients) (4). The TKE (k) is a real thing, because it can be measured directly. And it can be expressed as % of turbulence level, relative to the mean flow. You can use the actual measured data or assume a reasonable value. Anyway, you have direct control of it. (5). With the TKE (k) given, the eddy viscosity can be computed through the definition, if the dissipation of TKE is known. They are inversely related. Since the TKE dissipation (epsilon) is unknown, the eddy viscosity is also unknown. (6). But, what is the eddy viscosity? It is used to give you the Reynolds stresses through the eddy viscosity concept, if the velocity field is known.( the Reynolds stresses are related to the gradient of the velocity field.) The eddy viscosity is like a variable scaling factor. (7). Since the TKE dissipation is inversely related to the eddy viscosity, it is also just a variable scaling factor. (8). Now here is the interesting thing. At the inlet, there is a core flow region where the velocity is uniform (most of the time), and there is also boundary layer region next to the wall (unless the inlet is located at leading edge of the wall, there is always a wall boundary layer there). (9). For the thin boundary layer case ( assume that the thickness is zero), you have only uniform core flow region. The velocity is uniform, the velocity gradient is zero, and the Reynolds stresses are also zero. What is the eddy viscosity distribution ( or the TKE dissipation) for this uniform inlet flow? The answer is it can be anything, because any value times zero velocity gradient will give zero Reynolds stresses. In his case, it doesn't matter, you can give it any value. If the TKE dissipation is any value, then the length scale related to it can be any value. (But normally you just set it equal to the inlet diameter or a fraction of it.) (10). There is a serious problem here. If the pump is connected to a long pipe, then the inlet condition will be more or less fully developed flow. The Reynolds stresses for the fully developed pipe flow is not zero. I think it is a linear distribution. In this case, you have to reproduce the fully developed pipe flow conditions at the inlet. (11). And the eddy viscosity distribution ( or the TKE dissipation ) must be consistent with the fully developed flow solution. (12). If the inlet condition has a finite thickness boundary layer and a uniform core region, what are you going to do? The answer is: you have to specify the eddy viscosity, TKE dissipation and other variables in such a way that the finite thickness boundary layer can be reproduced at the inlet. In the rest of the core region, it is up to you to set the length scale. But I would use a number which will provide a smooth curve from the wall boundary layer side. In this way, the length scale distribution will be smooth and continuous across the inlet. (13). One can use the traditional mixing length distribution in the boundary layer as a starting point to calculate the length scale for the TKE disssipation. (14). As you see, setting the inlet condition is not just fixing a number, it is much more involved. In many cases, you probably have to solve the inlet pipe flow first, then use it as the inlet condition for the pump flow calculation. (15). If you don't set the inlet condition properly and realistically, you will get different results for your pump flow. Remember that internal flow is always much more difficult to solve than the external flows because the inlet condition is always non-uniform. Setting a number is not going to work.
  Reply With Quote

Old   July 2, 1999, 21:34
Default Re: length scales at inlet for internal flows
Duane Baker
Posts: n/a
Hi Anne Marie,

Quickly and pragmatially,

1. Typical dissipation length scales are from 0.1 to 0.5 (actually 0.41 which is Von Karman's constant....but I said that I was going to be pragmatic here!) of the spanwise dimension......I believe this is in the TASCflow docs. If you read the tutorial on turbulent flow in a duct, the example for turbulent flow in a duct of transverse L=0.3[m], the recommended L_{epsilon}=0.03[m].

2. The k-epsilon model is RELATIVELY insensative to upstream values of k and epsilon. The k-omega and some of the differential Reynolds stress models are NOT! See Wilcox's book, etc. for a discussion of this!

3. If one knows the rough geometric details of the upstream flows (as is normal in hydraulic turbine analysis) a coarse grid solution of the upstream stages can be solved and used as a BC for the domain of interest. The resulting solution of the downstream stage should be relativly insensitive to the upstream condition on the upstream stage!

Good Luck.........................................Duane
  Reply With Quote

Old   July 5, 1999, 21:28
Default Re: length scales at inlet for internal flows
Posts: n/a
Here is a check you should perform: Calculate the turbulent viscosity from your ke and diss boundary conditions --> mut = ke * ke * Cmu * density / diss (see your commercial code's user manual)

Then ratio mut over the laminar visocisity (mu). This ratio can give you an indication if your diss is resonable. If the ratio is say 10 or less, you do not have very turbulent flow. (Maybe realistic, maybe not) If the ratio is a million, you are trying to push "molasis" through your device - and probably will not get a converged solution.

For most of the applications I have modeled over the last 10 years, I actually assume an intensity, calculate a KE, assume a vis ratio (typically 100 to 1000) and back out a dissipation. Perform the initial run. Next test the sensitivity of the assumptions by increasing the vis ratio and/or the intensity. (These subsequent runs usually converge more quickly than the first run as I have a very good initilization.) If my result is sensitive to the inputs, you typically have to keep on moving "upstream" in your modeling efforts.

I also recommed plotting the viscosity ratio when you are doing your post processing to learn what "typical" ratios are in different situations.

  Reply With Quote


Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On

Similar Threads
Thread Thread Starter Forum Replies Last Post
Species mass flow inlet lorenz FLUENT 3 March 15, 2012 07:26
Validation 12.1 vs 6.3, Difference in Reported Inlet Total Pressure jola FLUENT 1 May 5, 2011 14:33
Inlet turbulent boundary condition, external flows ROOZBEH Main CFD Forum 1 February 6, 2009 12:37
mixing-sensitive reactive flow - subgrid scales Ingo Meisel Main CFD Forum 4 June 25, 2004 15:39
time averaged heat transfer in oscillating flow Matthieu Ubas Main CFD Forum 2 November 5, 1999 14:20

All times are GMT -4. The time now is 09:00.