open TELEMAC-MASCARET The mathematically superior suite of solvers

Hello everyone

I’ve some difficulties calibrating the evolution of thermal stratification in a lake and I think it’s due to excessive numerical diffusion. I would be thankful for any hint or advice!

The stratification is defined with constant level planes in “CONDIM”. I’m using Tel3D v7p2 cou-pled with “WAQTEL”. I intent a calibration of the stratification evolution when there is no inflow for a later use as reference state.

The calculation succeeds but the heating of the water body is still much faster as in the measurements, especially in the lower layers. For the beginning I’m not taking wind, rain and evaporation into account. In the model the heating of the lower Layers (4°C) happens within 6 days in model which is way faster than the measured heating over the summer (within 4 Month) in the measurements.

To make sure it is not due to the weather influence I made a calculation with a realistic weather and one with a constant weather with a temperature of 15°C as in the upper Layer of the stratified lake. In both cases the heating of the lowest Layers is too fast (see pictures at-tached) even if it happens a bit slower in the case with the lower temperature of 15°C.

The lake is about 1 km long, 100 m large and 10 m deep and I only found examples of way bigger stratified lakes. There may also be an influence of groundwater, since the lake is right next to a river. I assumed that this last point can’t be the reason of the high difference between the model and measurement. That’s why I think the model is still not really calibrated and there is still too much numerical diffusion left.

This leads me to following question: Is it possible to obtain a sufficiently low global diffusion (defined diffusion + numerical diffusion) to calibrate heat exchange with atmosphere in a rela-tive small lake as described?

In view of reducing the numerical diffusion as much as possible I already followed advices I found in different topics of the forum. The main changes I did are:
• I tried different turbulence models and got by far the best results using K-Epsilon.
• Refining the mesh a mesh size to 3-5 m instead of 5-8 m in the horizontal and 0,5 m instead of 1 m in the vertical (25 layers) improved the results.
• Augmenting the time step from 1 second to 8 seconds improved slightly the results
• “HYDROSTATIC INCONSISTENCY FILTER = YES” improved the results
• Varying “SCHEME OPTION FOR ADVECTION OF TRACERS “did surprisingly not make any difference
• I got slightly better results using the advection scheme 14 instead of 1
• Reducing the values of the diffusion coefficients for tracers (from 1.E-6 to 1.E-15) did not make any big difference in the results.
• Changing the accuracy for solver and diffusion of velocity, K-Epsilon and tracer (from 1.E-6 and 1.E-12) did slightly improve the results.
• Varying the calibration parameters of WAQTEL work as expected in the upper Layer (the heating in the upper layers becomes more or less sensitive to air temperature ac-cording to the values set) and is not the cause of the “fast” heating of the lowest layer.
• Varying “DISPERSION ALONG THE FLOW” (1.E-2 to 1.E-12) in waq_steer.cas did not make any difference

The exact settings can be found in the attached .cas file. At this point I do not have any idea of how to further improve the model. Has anyone an idea of what I could try to reduce the numerical diffusion?

In the attachment you can find some pictures of the initial condition and the actual results, the actual .cas file I’m using and also the actual fortran file.

Best regards
Peter

Hi,

usually, the numerical diffusion is mainly related to the advection of the velocities. Hence, the only really influential solutions are further refining the mesh or / and you can try also the ERIA scheme, which is the advection scheme nr. 15. This should be the less diffusive scheme. I tested it only in Telemac-2D. I don't know if it works in Telemac-3D. The developers should know more. You can switch on for the velocity and the tracer. For k and e a first order scheme is usually enough, like nr. 14.

Other things:
I would stick to default values for the diffusion coefficient of velocity and tracer (1.e-6) since they represent the kinematic viscosity of water.

Friction:
You set FRICTION COEFFICIENT FOR LATERAL SOLID BOUNDARIES : 1. which is 1 m..
You uncommented FRICTION COEFFICIENT FOR THE BOTTOM.. default value = 60 m. or do you have the friction coefficients in the geometry file?

Try to set mass lumpig to the default values.
Try to lower the IMPLICITATION FOR VELOCITIES to 0.55.

k-epilson model:
can be really very tricky to set up the inlet conditions in 3D. Depending on the prescribed boundary conditions for k and e and your geometry either you have too low k and e for a long stretch or you have too high values. If you have a geometrical disturbance in the vicinity of the inlet, then this disturbance will control your k and e downstream which is good. Otherwise you need maybe a really long stretch till the turbulence is fully developed, independently of the prescribed values for k and e at the inlet.

Hope this helps,
Clemens

Hi,

Thanks a lot for your help!

“usually, the numerical diffusion is mainly related to the advection of the velocities. Hence, the only really influential solutions are further refining the mesh or / and you can try also the ERIA scheme, which is the advection scheme nr. 15. This should be the less diffusive scheme. I tested it only in Telemac-2D. I don't know if it works in Telemac-3D. The developers should know more. You can switch on for the velocity and the tracer. For k and e a first order scheme is usually enough, like nr. 14.”

Unfortunately the computation doesn’t run with advection scheme nr. 15.
Concerning the mesh, I made a computation with a resolution of 0,25 m instead of 0,50 m to see if the results keep getting better with refining the mesh in the vertical. The results actually get better, but the diffusion of the tracer in the lower layer still happens too fast. A finer resolution in the vertical doesn’t seem reasonable to me for this case.

“Other things:
I would stick to default values for the diffusion coefficient of velocity and tracer (1.e-6) since they represent the kinematic viscosity of water.”

I changed it; of course it is still better to stay in the physical realistic, and as said before the effect of the results is quite meaningless.

“Friction:
You set FRICTION COEFFICIENT FOR LATERAL SOLID BOUNDARIES : 1. which is 1 m..
You uncommented FRICTION COEFFICIENT FOR THE BOTTOM.. default value = 60 m. or do you have the friction coefficients in the geometry file?”

No, I do not have the friction coefficients in the geometry file.
I corrected the values and set them = 0.03.
It didn’t change the results since there is no inlet in this calculation. But it would have be an issue in the further calculations with an inflow.

“Try to set mass lumping to the default values.”

“Try to lower the IMPLICITATION FOR VELOCITIES to 0.55.”
This actually made the results a bit worse.

“k-epilson model:
can be really very tricky to set up the inlet conditions in 3D. Depending on the prescribed boundary conditions for k and e and your geometry either you have too low k and e for a long stretch or you have too high values. If you have a geometrical disturbance in the vicinity of the inlet, then this disturbance will control your k and e downstream which is good. Otherwise you need maybe a really long stretch till the turbulence is fully developed, independently of the pre-scribed values for k and e at the inlet.”

Thanks a lot for these informations concerning k-epsilon model, I will keep that in mind for the computation with an inflow.


Best regards
Peter

Hello everyone.
I was reading your post and I would like to ask some questions; because I am trying to calibrate thermal stratification in a reservoir too; first, at all, I want to know, with which tool do you visualize the temperature results, I trying my self with postel3D, but I dont have all my planes.
And second, I have the same temperature for my reservoir.
So I don't know if the time is not enough or if my setup is no good one.

Hello everyone.
I was reading your post and I would like to ask some questions; because I am trying to calibrate thermal stratification in a reservoir too; first, at all, I want to know, with which tool do you visualize the temperature results, I trying my self with postel3D, but I don't have all my planes.
And second, I have the same temperature for my reservoir.
So I don't know if the time is not enough or if my setup is no good one.
Thank you very much

Hello everyone.
I was reading your post and I would like to ask some questions; because I am trying to calibrate thermal stratification in a reservoir too; first, at all, I want to know, with which tool do you visualize the temperature results, I trying my self with postel3D, but I don't have all my planes.
And second, I have the same temperature for my reservoir.
So I don't know if the time is not enough or if my setup is no good one.
Thank you very much