open TELEMAC-MASCARET The mathematically superior suite of solvers

Hi

I am simulating flow over bed forms using TELEMAC 3D. I tried defining my own distribution of the levels with additional refinement near the bed surface using the CONDIN subroutine (MESH TRANSFORMATION=2).

When I run this my velocity profile is constant in the vertical direction. When I run with the homogeneous distribution (MESH TRANSFORMATION=1) I get a proper vertical profile(see attached my files for this case).

Is there something I am overlooking? Thanks very much for any help.

Cheers
Patrick

Hello Patrick,

This case is really interesting. Would you have an analytical solution for it ? I seem to remember having seen one somewhere in the literature. If you do have one, would you mind if we include this case in our validation set ?

To answer your question: indeed the profile is constant with MESH TRANSFORMATION set to 2. I cannot see any problem with your setting, so you may have here highlighted a problem with TELEMAC. The only thing I can think of is that ZSTAR(2) is too small to be considered separate from ZSTAR(1), and as a result the bottom friction may not be applied properly. This requires further investigation (by EDF principally?, Jean-Michel, Chi-Tuan, can you have a look?) as a threshold value needs to be modified to an even smaller value.

To confirm this, I have done a test where the first 10 values of your ZSTAR table are simply (0.D0;0.02015D0;0.03117D0;0.04394D0;0.05933D0;0.06822D0;0.07149D0;0.08001D0;0.09465D0), and it works (I do get a proper velocity profile).

Hope this helps.

Sébastien.

Hello,

I have investigated your case and I first would like to be sure that you want to prescribe elevation both at the entrance and the exit of your domain (code 5 4 4 in the boundary conditions file).

Regards,

Chi-Tuan

Hi Sébastien and Chi-Tuan

Thanks for helping me with this problem.

This problem I am working on is to examine dune evolution - so my first step has been to model uniform flow over dunes. This dune shape (400mm long by 20mm tall) is common and found in a number of papers (I can send you a list if you want). I dont have an analytical solution for this case, but the following thesis contains experimental data that I am using to validate my model.

Polatel, C. 2006. “Large-scale roughness effect on free-surface and bulk
flow characteristics in open-channel flows.” Ph.D. thesis, Iowa Institute of Hydraulic Research, The Univ. of Iowa, Ames, Iowa.

I was using this high-resolution mesh to see if it would resolve problems I was having with the flow separation on the leeside of the dune. As you mention, this mesh may be a little too fine. I have another lower-resolution geometry (dx=10mm, 20 planes)consisting of 12 dunes which is giving better results.

With regards to the boundary conditions, I had initially perscribed a flow at the upstream boundary condition but found it created to instabilities at the inlet. It was recommended that I try specifying elevations at the upstream and downstream boundaries and this seems to eliminate the instabilities I was having.

Thanks again for taking time to help me with this.

Cheers
Patrick

Hello,

I think it should work only with a discharge prescribed at the entrance (and free elevation). It works with many test cases (including the dune problem) and there is no reason why it should not work here. Your case with elevations at both sides is not well posed, and you do not prescribe velocities, so the velocity profile you find is the result of the computation, not what you ask through keywords.

It is important to give the discharge, not the velocities. If you give velocities with free depth your discharge will vary in time, and in this case you may have waves going down, reflecting on the exit with prescribed elevation, and then going back (it is a very amazing and interesting effect but not exactly what you want).

With best regards,

Jean-Michel Hervouet

Hello Patrick,

I'm only curious because we have a similar physical model here and are doing comparisons with a 3-D code. Why in your case do you use the Smagorinsky model for modelling the turbulence?

Best regards,
Clemens

Hi Patrick,
sometimes the convergence of this kind of problems requires a "hotstart" from a base solution.
If you still have problems following JMH's suggestions I'd recommend you to try to run your simulation starting with the same channel, same flow conditions (see JMH hints) and closure models but without the dunes. This will give you an idea of the "behaviour" of your solution.
As a second step, you can try to run your test with dunes.

I hope this help.

best, pablo

Hi Everyone

Thanks again for your helpful comments.

I will switch my upstream boundary to a flow condition and use a hotstart - the idea of using a flat-bed first is also a great idea. Thanks for these suggestions. My current model is a train of 12 dunes on a 1/700 slope to allow the vertical profile to develop and stablize.

With regard to my choice of vertical turbulence model, I was running the model with all of the turbulence models. The one I posted just happened to be the Smagorinsky model. I was comparing the results using the different turbulence models against the experimental data to determine the best model to use. I admit that turbulence modeling is something I do not have much experience with. I will be taking a course in it next term. In the meanwhile would appreciate any suggestion on which model would be most appropriate for this problem.

Cheers
Patrick

Hi Patrick,

I just read your posts. I hope it is not to late for some hints.
I am doing dune modelling (but with morphodynamics) as well.
Wich Telemac Versiona are you using? I used a very fine mesh at the bottom as well, with ZSTAR2 = 0.00138 with version v6p0. This worked fine, but the newest version v6p1 can't handle this fine meshes close to the bottom. I needed to change that in order to make it work.
Also maybe you should use a mesh that is less distorted (in the horizontal)? Your triangles have very low and very different angles.

cheers
Annalena

Hey Patrick,
your model gets your desired mesh distribution, if use the princi file I attached below.
good luck
Annalena