open TELEMAC-MASCARET The mathematically superior suite of solvers

Hi,

I am a new user and would like to know how to use Telemac first. I would like to perform 2D simulation for urban area with considering buildings. I am trying to do a model based on pluie training case. I have a DEM with 1 m resolution. I reduced the DEM resolution to 10 m and imported it to BlueKneue. Then, I created the mesh, interpolated the elevation to it using the inverse distance method. Afterwards, I defined the bottom, bottom friction and CN (I used one number to all my study area for simplicity).
I checked the Pluie example and tried to create a file based on it. I defined the CN in the mesh and the rainfall as a hyetograph in a formatted data file.

I would like to ask the following questions:
- what does the ''NUMBER OF PRIVATE ARRAYS = 4'' in the Steering File means.

- What is the Fortran file in the input/output files (FORTRAN FILE ='t2d_pluie_cn_geo_hyetograph.f')?

-I created the boundary condition file but didn't define any boundary condition as I don't have any gauge or source of water ( I am working on urban area and would like to perform rainfall-runoff model). However, when I checked the files from Pluie example, I found that there is a boundary condition file. Thus, I just created the file.

When I tried to run my model with the attached files, all results are zeros.
I would be grateful if someone can check the files and explain for me my mistakes.
Please inform me if the file is not shown in the attachment.

Best regards.
Omar

Hello!

I have looked at your case and there are a couple of things you need to improve.
First of all, you have a friction coefficient given in your mesh file which is 0.06 which seems relevant if you use the Manning friction law. In your steering file you however use Strickler's law (LAW OF BOTTOM FRICTION =3), so a Strickler coefficient of 0.06 is extremely low creating a HUGE friction. That's why water is not moving your results. The Strickler equivalent of Manning 0.06 is 1/0.06 = 16.67.
I checked your results and it's not zero. You maybe need to activate the option "Animate" in Blue Kenue to browse through the different time records. At time = 0, most part of the results are zero indeed.

For your questions:
NUMBER OF PRIVATE ARRAYS = 4 is set in this case for two reasons:
1/ to be able to read your user defined CN in the mesh
2/ to be able to save extra user variables in the result file. This was done mainly for validation purposes, you don't need those extra three variables in your results (CN COEFFICIENT, ACC. RAINFALL, ACC. RUNOFF).

Fortran file. This is a general TELEMAC feature that allows the user to modify parts of the code to make some changes. In this specific case, changes are needed to the runoff_scs_cn.f subroutine to allow:
- reading the CN coefficients from the mesh
- reading and interpolating the hyetograph data

I suggest you read the user manual and look into several validation cases to become more familiar with this feature and how/when to use it.

Lastly, beware that the steering file you use was set up for testing purposes on a schematic mesh. The numerical set-up needs to be changed in you want to model real world cases (time step, turbulence etc.). In some cases, it is even better to perform rainfall simulations in finite volumes rather than finite elements (default method).

Hope it helps,

Kind regards
PL

Hello Pilou

Thank you for your kind response.
I checked my file and it works now.
I started with performing the simulation with finite element and it is working, however, the courant number is too big. I used time step 60 sec and I think that is the reason so I am running the model now with 1 sec and waiting for the result. the model is slow but I think that my time step is small and I should increase it as the model perform the calculations within 9-10 iterations and I think that the ideal is between 20-40 iterations.

As you recommended, I tried to perform the simulation based on finite volume by using the following options:
FINITE VOLUME SCHEME =1
TIME STEP =1
VARIABLE TIME-STEP =YES
DESIRED COURANT NUMBER =0.9
EQUATIONS= 'SAINT-VENANT VF'

I got an error that the tidal flow should be True. The model run when I delete EQUATIONS='SAINT-VENANT VF'but I don't know now if my model is based on finite element or finite volume as I think that EQAUTIONS='SAINT-VENANT VF' is the command that makes the model ignore all the Finite element parameters in the simulation. I added the steering file in case you would like to have a look at it.
Thanks in Advance

Hello!

Try the HLLC finite volume scheme, I found it to work well for rainfall modelling. FINITE VOLUME SCHEME =5

You are right, a lot of the standard numerical settings are actually specific to finite elements and not valid for finite volumes. You will also find that finite volume are much slower than finite elements but I think finite volumes is the way to go for rainfall modelling, mainly due to the fact that they can handle very small water depths and tidal flats much better than finite elements.

Kind regards
PL

Hello,

Thank you for your prompt response.
I perform the model based on both FINITE VOLUME SCHEME =1 and FINITE VOLUME SCHEME =5 and there is almost no difference in the resulted water depth (is it normal?) but the model is giving me the error message as shown in the attached image when I perform the simulation based on the Finite Volume.
When I remove the EQUATIONS ='SAINT-VENANT FV' from the file, the model runs normally. I would like to ask for the following:

1- By removing the EQUATIONS ='SAINT-VENANT FV' from the file, is the model perform the simulation based on Finite Element as I already stated that FINITE VOLUME SCHEME =5 or it perform it based on Finite element.

2- I controlled the courant number to be less than 0.9 and the time step to be variable to make sure that the simulation is stable. I read in the user manual that these options are to be used with the Finite Volume method but is it possible to use them also with the Finite element method?

3- I attached my selfain file and will be grateful if you can tell me if there is any option to add to run the model normally without getting the error, I already activate the tidal flats option so I don't know what to do.

Thanks in Advance

Hello,

Oops, this is a bug left in subroutine prosou_fv.f (tidal flats is only used in finite elements and this section has been left in this finite volume subroutine due to a simple copy/paste mistake). Add this subroutine in your fortran file or fortran folder and comment out the following section (example below is taken from version 8.1, from line 387 in prosou_fv.f):


Hope it helps!

Kind regards
PL

Hi,

Thank you for your kind response.
I installed TELEMAC v8p1r0 however I couldn't find the prosou_fv.f in the subroutines folder. I only found only the prosou.f file and I attached it. I added it to my Fortran file and commented out the same section as you recommended. However, the model is working but not correctly. It performs the simulation in 3 mins and the result file is empty.
I would like to ask if you have a reason why the prosou_fv.f is not included with my TELEMAC version.

Hello,

This is strange. I also have v8p1r0 and prosou_fv.f is in the sources/telemac2d folder. There is no reason why the file should be missing and you wouldn't have been able to compile the code. Double check, maybe you looked into another folder?

If your problem with no results still persits please post your case with all files here, I can have a look.

Kind regards
PL

Hello,

Thanks for your reply.
I reinstalled TELEMAC again on my laptop and the new one has the prosou_fv file, probably I did something wrong while installing the program for the first time.
When I run the model based on the finite volume method, the model run without any error. Thus, I didn't modify the subroutine.
I run the model on a more fine mesh (1m) as my previous model was based on 5m mesh. However, my laptop restarted while performing the simulation, according to the TELEMAC manual, I continued the simulation by using T2DRES file to get the previous time step data by adding the following lines to my selfain file:
COMPUTATION CONTINUED =YES
PREVIOUS COMPUTATION FILE ='T2DRES'
the model continued the simulation however I noticed that the following:
my original precipitation is 50 mm distributed on the first 6 hrs of the simulation and I am continuing my computation from the 6hr which means that the model already got all the precipitation and will not add any more precipitation but when I continue the computation, the model continues from the next time step but it is adding more precipitation to the simulation as shown in the attached image.



After continuing the computation, I noticed also that the accumulated rainfall is increasing but the water volume in the domain is constant which is not logic.



I would like to ask if you have an explanation for it.

Hello,

Unfortunately, the rainfall-runoff model implemented in runoff_scs_cn.f does not handle hotstart procedure (COMPUTATION CONTINUED), the arrays where initial and continuing abstractions from the CN method are always initialized to 0 at the first time step of a simulation, even in case of restart. This is why you see that the volume within the model is kept constant just after the restart while precipitation increases: the first part of the precipitation is catched and lost in the initial abstraction Ia, giving zero runoff (and therefore volume).

A custom initializating could however be done from within the subroutine but this would need some testing (I don't have a solution that works immediately for this).

So I am afraid that the only solution is to re-run the model from scratch.

Kind regards
PL