open TELEMAC-MASCARET The mathematically superior suite of solvers

Dear community,

I'm trying to simulate a measured time-series of water surface elevation in a semi-enclosed basin (part of the Baltic Sea).
My idea was to generate a modelled signal of water levels, only driven by a measured windfield and to compare this to the measured water level signal.

As tides here are neglectable I excluded this factor for now. However, the simulated signal is not even close to the one which's measured.

I've run the simulation on the basis of a certain time-series for a windfield. At the moment I'm wondering if I need to provide also a water level time-series as an additional driver for the simulation. So there is also a prescribed elevation provided.
As far as I read, for doing this, I need to adjust the 'condin' subroutine to indicate the location of the gauge where the water level was measured and to provide the time series. Is that correct?

And, does is there any instruction on the use of the subroutines? I'm not familiar with these and haven't use one yet.

Many thanks for any recommendations,
cheers Tim

Hi everyone,

as far as I found out there is no real option to define the liquid boundary by, geographically, just one single point/hydrograph. As far as I understand I can define the LIQUID BOUNDARIES FILE for the open boundary which then should use these values all over from this certain location.

I prepared a time series of water elev. from that hydrograph and made my meshs' open boundary close to the location; to get a best fit.

However, there seems to be something wrong with my LIQUID BOUNDARIES FILE as I get the message: BAD REAL NUMBER IN ITEM 1 OF LIST INPUT.
The first Number is a negative decimal num. which I actually wouldn't change as this would in principle change the time series.
I've looked up some of the examples and found that most cases have e.g. SL (SeaLevel) and some other variables like velocity or discharge etc.

I'm wondering if need more than one variable?

I've posted my log-file with the error as well as my .lbf in the attachment.
Any help is much appreciated.
Cheers Tim

Hello Tim,

Can you upload your LIQUID BOUNDARIES FILE, but e.g. a .txt extension as not every extension is allowed.
Can you also share your steering file + boundary conditions file please?

FYI the CONDIN subroutine is only used to define initial conditions.

Chi-Tuan

Hi Chi-Tuan,

thanks for reaching out. Please find attached the mentioned files. I've also added the geometry file.

Regarding the CONDIN, thanks for the explanation. Does telemac initialises the conditions from the LIQUID BOUNDARIES FILE or do I have to forward the computation via the CONDIN to the LIQUID BOUNDARIES FILE?

At the moment I don't understand how the model initialises the setup without prescribed information. I've the feeling that I'm missing some point.

Cheers, Tim

Hello Tim,

There is a problem with the format of your LIQUID BOUNDARIES FILE: there must not be empty lines, that is why you should have gotten this error message.
Moreover, ban the use of tabulations with ASCII files, in particular this kind of input files and Fortran files.

LIQUID BOUNDARIES FILE is used to prescribe boundary conditions.
As told, CONDIN computes initial conditions.
Initial and boundary conditions are defined separately.

If not already done, I strongly recommend you to read the TELEMAC-2D user manual available on this website: wiki.opentelemac.org/doku.php?id=documentation_latest
or directly with the sources in
$HOMETEL/documentation/telemac2d/user folder.

Hope this helps,

Chi-Tuan

Hello Chi-Tuan,

first of all, thank you for your help! I edited the LIQUID BOUNDARIES FILE the way you suggested. I did read the manual but wasn't clear about the files being so sensible to tabulations.

I did work on several model setups over the last weeks, trying to get the forcing/boundary conditions right to represent a hydrograph in the inner fjord. I managed to represent the asked surface elevations of the hydrograph by forcing the model using only another hydrograph on the models' outer edge at the open boundary; which was the time series of my .lbf. The results were reasonable and the match of good quality.
From my deliberations, this seems reasonable as the surface elevations of my .lbf time series is a result of real-world wind-driven changes in surface elevations. So far so good. Tides are neglectable in this case.

However, thinking it the other way around I'm now trying the model to represent the inner fjords surface elevations by forcing it with only the relevant wind conditions; neglecting/not using the .lbf time series in this case.
Imagine you have only relevant wind data, and one time series of a hydrograph to validate the model against. It should be possible to represent the measurements somehow close.

I have the feeling my wind setup is not quite right. What I get is, either my domain is emptied almost completely and then one can see some wind-driven oscillations of the surface elevation for the model runtime, or there happens hardly anything in terms of changes in elevation. The second is the case when I use COEFFICIENT OF WIND INFLUENCE VARYING WITH WIND SPEED.

The documentation for wind forcing is not really sound, so would be great if you have any advice. I added my steering file in the attachments, in case you want to have a look.

kind regards,
Tim

For a better understanding, I produced two graphs showing the surface elevations including a "coefficient of wind influence varying with speed" and the model outcome without the variations.

Hello Tim,

I am not sure to have all understood what you wrote.

Would it be possible to upload the BOUNDARY CONDITIONS FILE = Vali_BC.cli you used for your last computations please? In particular, I would like to see what kind of boundary conditions you use.
But also your ASCII ATMOSPHERIC DATA FILE ='t2dRAD201122-29'

What is the size of the elements (min and max) and the expected velocities over the domain? What about the water depth expected?

Some first comments about your steering file:
I am not sure using the keywords VARIABLE TIME-STEP and DESIRED COURANT NUMBER work well when using Finite Element method in TELEMAC-2D.
You use OPTION FOR LIQUID BOUNDARIES = 2 i.e. Thompson boundary conditions, but for your open boundary, is it really what you want?

Chi-Tuan

Hello Chi-Tuan,

thanks for reaching out again.

I'm trying to represent the surface elevation time-series from the hydrograph near Holtenau. At the moment I try to do this by having wind as the only forcing. The data I use is the mentioned time-series of the Holtenau hydrograph and wind-data from the local airport for the same time window. I've attached a map for a better geographical understanding.

Until now I managed to get a good representation of the Holtenau hydrograph by forcing the model with a surface elevation time-series from the Kiel-LH (lighthouse) hydrograph. Changes in surface elevation are dominated by wind-driven currents in this region. Therefore so far the results seem reasonable to me as also the measured surface elevations at Kiel-LH incorporates the wind, respectively are results of the wind-driven currents.

However, as my further studies rever to more local currents in the inner fjord, e.g. set up by different wind conditions scenarios, I want the model to represent measurements by having actual wind data as driver/forcing and not the hydrograph at Kiel-LH.

You can find my BOUNDARY CONDITIONS FILE in the attachments, as well as my ASCII ATMOSPHERIC DATA FILE. My open boundary is set up for a prescribed H. I haven't changed it from my run forced by the Kiel-LH hydrograph.

The elements sizes are min. 119m2 and max. 202589m2. As the run forced by the Kiel-LH hydrograph gave reasonable results, the read velocities of this are up to 3.88m/s. The expected water depth is up to 22,90m.

The VARIABLE TIME-STEP is commented for the reason you mentioned (it's a relict as I copied the steering file from a former project), do I understand you correctly that I should comment the DESIRED COURANT NUMBER as well?

Actually, I'm not sure about the Thompson boundary. I was thinking that, when I impose wind data on the model, this option would "suggest" a reasonable surface elevation at the open boundary; as mentioned in the manual. Especially as I chose a prescribed H open boundary and implemented an INITIAL ELEVATION in the steering file.

Cheers,
Tim

Hello Tim,

I think the 1st problem is that you set prescribed depth for the open boundary (code 5 4 4) and you do not fill PRESCRIBED ELEVATION keyword or give a LIQUID BOUNDARY FILES. In that case, the water depth to be prescribed is considered constant in time and space and read from the BOUNDARY CONDITIONS FILE (in your case, it should prescribe a water depth = 0 at the open boundary, you can check if it is the case or not, that should happen with classical boundary conditions with OPTION FOR LIQUID BOUNDARIES = 1, not 2 aka Thompson conditions).

With Thompson boundary conditions, the water depth at this open boundary should not be so different from 0 I guess. Thompson boundary conditions will solve the boundary conditions by combining water depth and velocity suggested, but not the wind I think.

I have a few questions about the area, that may help you to prescribe a better boundary condition:
- what is the influence of tide there (I am not a specialist of the Baltic Sea)?
- does free surface elevation move a lot at the open boundary? What tidal range can be expected?
- to what reference level is the bottom elevation refered to? Mean Sea Level? Chart Datum? Something else? If MSL and no big effect of tide, a mean value of 0 may be OK,
- do you have atmospheric pressure data available? Maybe you can add an inverse barotropic effect to the predicted water level? If wind is strong (due to storm surge e.g.), its effect can be modelled by this means at the open boundary.

But I think you have to solve the boundary condition first prior to tune the wind effect.

Anyway, if you unset VARIABLE TIME-STEP, the keyword DESIRED COURANT NUMBER should not be used. But it is easier to read steering files without unnecessary keywords.

Be careful with the time step. Be sure it is not too big for the velocities and size of elements.

A last comment about the value of the CORIOLIS COEFFICIENT. I am not sure that it is so small at Kiel latitude. Please have a look at the T2D user or reference manual.

Hope this helps,

Chi-Tuan