open TELEMAC-MASCARET The mathematically superior suite of solvers

Hello,

I have some questions or remarks regarding the entrance condtions at liquid boundaries for the turbulent kinetic energy k and its dissipation eps.
From version v6p3r2 to version v7p0r0 the boundary conditions for k and eps in case of liquid boundary have apparently changed, see kepcl3.f. Good to know.

According to the lines 269 and 319 in kepcl3.f the approaches by "HANS AND BURCHARD or "Hans et Burchard" are adopted. Who is Hans and who is Burchard? However the internet gives a researcher named Hans Burchard.
So I would be glad if anyone could give me the reference paper for this implementation.

In line 241 Z0 is defined as RUGOF%R(IPOIN2)/30.D0, which is then used as limiter in the computation for EBORL at the liquid boundary in line 321. So I think if the user specifies a friction law other than the Nikuradse law some problems may appear?

Did anyone test the new boundary conditions for some different cases? I ran it with the rectangular channel bump validation test case and when inspecting the results the TKE and eps results seem really weird.

And it would be cool if such modifications are announced also in the "What's new" section.

Best regards,
Clemens

Hello Clemens,

Yes, you are entirely right, this was actually an unexpected byproduct of another development, which was not really discussed. I would prefer keeping the previous version that consisted in giving no turbulence at the entrance, or adding a keyword to decide whether we want nothing or another formula like Burchard (I have no reference to give but know who to ask for that). The results of a test case on stratification were also subsequently changed and lost part of its meaning.

I'll discuss rapidly with my colleagues whether we should remove Burchard as default in version 7.1 (now due for 23rd December).

With best regards,

Jean-Michel Hervouet

Hello Jean-Michel,

thank you for the answer. Some other remarks:
actually the implementation is reasonable since it assumes simply a linear decrease of k_bed and epsilon-bed from the bottom boundary condition (see e.g. Rodi) to the water surface with k-surf and epsilon-surf being zero at the surface. This description reflects the vertical distribution of k in open channel flow & log-velocity profile (lot of literature) and fits e.g. well to my measurements (hopefully written down soon )

As a side note and to get conform with the water surface condition and in order to avoid too high differences between adjacent nodes: if the user specifies a dirichlet condition at the surface for epsilon-surf (line 220 in kepcl3.f) the linear interpolation should be between those values.
And shouldn't have k and epsilon a Neumann boundary condition at an outflow boundary? See line 259 in kepcl3.f for k.

The THEORY BY VINCENT BOYER for the inlet condition, k as a function of inlet velocity and turbulent intensity, is the usual approach in various CFD packages for pipe flow simulations and there it works well. However in open channel flow and assuming a logarithmic velocity profile at the inlet the approach would give an increasing k towards the surface and so the channel distance needed for a physical (reversed) k profile would be maybe even more compared to a condition with no turbulence at the inlet.

So I would appreciate the idea, if the user can decide between the two options using a keyword. By the way in Telemac-2D the implemented inflow boundary conditions for k and epsilon work very well.


Best regards,
Clemens

Hello again,

some days ago I went into this investigation because i got really unphysical results for the turbulent kinetic energy and the dissipation with e.g. minima and maxima values (clipping values) in adjacent nodes and so on.

So far I didn' t get rid of this abnormal behaviour by inspecting the boundary conditions. However it has been a nice excursion.

Finding: the default method of characteristics as advection scheme for k and epsilon is the reason?!

Changing the advection scheme for k and epsilon - SCHEME FOR ADVECTION OF K-EPSILON - to e.g. 3, 4, or 14, I get the results what I expect!

And these findings apply also to the older version v6p3r2.


Best regards,
Clemens

Hi, me once again ,

I also have problems with the k-epsilon model in v7p1r0.

My simulations are running well with constant eddy or the Elder Model, but switching to k-e creates instabilities in the velocities and in the water level based on bouncing k and epsilon and corresponding dissipation implemented on the inflow boundary.

With very small time steps and mean flow, Telemac2D manages to smooth this bouncing variables out after 2km of free flow section, but there is no chance to model a flood wave or even higher discharges with k-e.

I tried the SCHEME FOR ADVECTION OF K-EPSILON = 14 and to my surprise I got the error
KEPSIL : Unknown type of advection:14

Maybe I do not get the link, but shouldn’t be option 14 available? Apparently there are just option 1 and 2 coded in kepsil.f……

So my questions:
How to get option 14 for k-e and why does the k-e model implement this bouncing stuff on the inlet boundary?

Many thanks,
Gabi

Hello again,

Yes, I looked at kepsil.f, and only characteristics and SUPG have been implemented. So I added this on my list again... In the while you can use the method of characteristics and it should not raise any problem (it is monotone even on dry zones). This advection of k and epsilon has probably nothing to see with your problem.

On inlet boundary conditions: in Telemac-2D we have put at entrances a theoretical turbulence due to a balance with the bottom friction. This is questionable and does not always work. You can change this and try to put a very small value of k and epsilon (this is to be done on kepscl.f, the values of KBOR and EBOR are k and epsilon at the boundaries). Small = 1.E-6 to 1.E-10, so that there is no turbulence at inlets (it is what we eventualy did also in Telemac-3D, because other possible formulas gave much too large turbulent diffusion e.g. with large depths). A drawback is that turbulence may take time to set up after the entrance.

With best regards,

Jean-Michel Hervouet

Hi Jean-Michel,

thanks you for the suggestion, I'll try it.

Regards,
Gabi

Dear Jean-Michel,

I followed your suggestion to modify kepscl.f and it worked for the boundary nodes, but 5-6 nodes downstream I got this wiggles in k,e,dissipation and velocities and water level again. About 1km downstream, the wiggles are smoothed out, but at the moment I have no idea where they are coming from (if it is not the advection).

I attached the time series of the turbulent energy and the plan view.

Best regards,
Gabi

The files

The red line at the time series is at the inflow boundary (set to 1E-6),
the blue one is approx. 5 nodes downstream, green and yellow are approx. 150-200m downstream, light blue is ~500m downstream