open TELEMAC-MASCARET The mathematically superior suite of solvers

Hello,

First of all, I would like to praise here.
The tememac-community is just right for such complex computational tasks.

For the N-A calculation of an 80km2 area I used the module Pluie as a pattern.

The result (that is, the depths of the water) seems realistic to me for the result.

RUNOFF_SCS_CN: TOTAL RAINFALL VOLUME ACCORDING
TO USER DATA: 65.916163471180909 MM


Only the amounts of water (Flux Boundary or Volume of the Domain) show incorrect values.

INITIAL VOLUME: 809308.8 M3
FINAL VOLUME: 0.2187435E + 08 M3
VOLUME THAT ENTERED THE DOMAIN: -0.4790588E + 08 M3 (IF <0 EXIT)
VOLUME ADDED BY SOURCE TERM: 2000925. M3
TOTAL VOLUME LOST: -0.6697000E + 08 M3

The INITIAL VOLUME is right 80,000,000 m2 x 0.01m Initial depth = 800,000m3
FINAL VOLUME + VOLUME THAT ENTERED THE DOMAIN is wrong: 80.000.000m2 x 0.0659m + 800.000m3 = 53.520.000m3

FLUX BOUNDARY 1: -1309.305 M3 / S (> 0: ENTERING <0: EXITING)
This value is too high. Values of 45m3/s are measured at the level.

Therefore my request:
Why does pluie calculate this extreme volumes in idf type rain?
Could look anybody here of my .cas files.
Something inexplicable to me seems to trigger these exaggerations.

my files oncloud:
download-stadt-raum.de.cool/index.php/s/7Zv3W82lUNTngPs

Hi!

Happy to see that some folks use the IDF relationship from runoff_scs_cn :)

I have a couple of comments. First of all you have a very coarse mesh for performing runoff simulations with element sizes up to 86 m. This combined with very shallow water depths is not a good combination for finite elements. Something is going wrong in your simulation, you have a complete rubbish mass balance. I would suggest you to try finite volumes instead (scheme 5 can be used in parallel) and to close the model at first to make sure that mass balance is achieved. Then re-open the downstream boundary. Eventually refine your mesh.

Then there is a second point that might lead to instabilities using IDF relationship. It has to do with the rainfall intensity potentially being near infinite just around the rainfall peak. To avoid this numerical/artificial issue I define rainfall intensity as constant during say 5 minutes around the peak, the actual intensity being calculated from the IDF parameters so that the total rainfall amount is unchanged. I will submit this change to the development team as I think it should be a default feature.

Here is the changed part, corresponds to lines 157-167 in your fortran file:

Make sure to declare DP variable PEAK_MINDUR at the beginning of the subroutine.


Hope it helps!

Kind regards
PL

Hello!

Thanks for the answer and the tips.

The IDF relationship in the form of a cds in the runoff_scs_cn is a bit more cumbersome, but in contrast to a block rain, the result is closer to the scs method, as it was once originally developed. :)

I have used your Fortran code to avoid precipitation peaks. It works, but the volume is still too high.

If I set the IDF values ​​calculated by me over a table at intervals of 10 minutes, the volume values ​​seem to me more plausible. Only the water depths are then too low. Probably because of the size of the grid.

And yes, my grid does not seem to be suitable for finite elements. However, I had the following conditions when generating the mash.

- in the water area: 1m point distance (high density)
- in the catchment area: arbitrary, since no water depths are relevant here.

If I generate a total area of ​​80km2 ideally at 1m point distance, I will get 160 million faces, which will exceed my computing capacity. Currently I have 2Mio partial areas, which is just acceptable for an office computer.

If I first close the model to ensure that mass balance is achieved, the calculation will abort with a #NV error. Probably because then everything is flooded.

One question: Did you mean to experiment with finite volumes (Scheme 5) that I should calculate the simulation with Telemac3d instead of 2d?

Hi!

I don't have the time to look into your case into detail but here are some further comments.

Why do you have initial conditions defined as a water depth over the whole domain? This is not a physically correct set-up for such a case and it might lead to instabilities.

Your rain in 3 hours long and your simulation time is 12 hours. The fact that you obtain crazy results at the outflow boundary at the end of the simulation indicates that the problem is very likely not linked to the rainfall set-up but rather to your mesh / boundary conditions / numerical set-up. The fact that your simulation crashes with no open boundary is no good sign either...

Modelling runoff can be tricky so I would suggest that you start with a simpler case (much smaller area, smaller element sizes) so that you can find which settings you need to use to have a stable hydrodynamic simulation without errors before increasing your model size (80 km2 is very ambitious though...). As I mentionned, and as highlighted in previous papers from the User Conference (look for 2016 and 2017), finite volume schemes are best suited for such a modelling. You can activate finite volumes in T2D with the following keywords (read the manual also):

EQUATIONS = 'SAINT-VENANT VF'
FINITE VOLUME SCHEME = 5
VARIABLE TIME-STEP = YES
DESIRED COURANT NUMBER = 0.8

Beware, it's much slower than finite elements so you need some cores to get acceptable CPU times for a real world case. I see that you are on version 7.2. Upgrade to 7.3 as there were some bugs with FV + rainfall in 7.2. I now use 7.3 and it works like a charm.

Finally, I don't understand what you mean with "If I set the IDF values ​​calculated by me over a table at intervals of 10 minutes, the volume values ​​seem to me more plausible. Only the water depths are then too low. Probably because of the size of the grid". The volume information given by

RUNOFF_SCS_CN: TOTAL RAINFALL VOLUME ACCORDING
TO USER DATA: 65.916163471180909 MM

is actually only a check using the given IDF parameters, look at the subroutine. The actual volume entering the domain (runoff, not rainfall) can be monitored with VOLUME ADDED BY SOURCE TERM (units: m3) or with the array ACCROFF from the subroutine (units: meters). You will of course never get 65.9 mm since you have abstractions and infiltration. You can use the test case pluie along with the SCS equations to check how the whole thing works.

Kind regards
PL

Hello pilou1253

Thanks for your answers. Your comments are very helpful to me. Anyway, I'm getting on the right way.

With the initial conditions as water depth over the entire domain, I originally wanted to define dry weather drainage from groundwater. The value of 0.01m is probably too high and causes the problem with high volumes. If I perform a calculation without initial conditions as water depth, then the extem values ​​disappear. Presumably, this is one of my problems with instabilities.
A definition of the rain over the IDF parameters or the SCS infiltration seems to me correct.

I also suspect that within the 80km2 areas such as Terrain troughs, quarries with too large areas are present which lead to these instabilities.

Although I am still busy in the next few days with other projects, but would like to follow your advice with a smaller model and finite volume version 7.3 with multiple cores happy.

I still have a little request: would it be possible for you to upload a working example with any ".cas" as well as a subroutine ".f" That would make it easier for me to find my mistakes. I could then at least a lot easier to understand.

I would also have a suggestion. Maybe one could here for example create an upload area where users can upload real projects and explain it. That would be a very good source of information for many users.

Hi!

For cas file, start from the pluie examples and just add the keywords required for finite volume at the end of the steering file (a lot of numerical options are specific to finite elements and are therefore not used with finite volume, such as turbulence for example).

Regarding the fortran file, I simply use the default version with the small changes I posted in my previous message.

Test it on a smaller area and it should be working just fine. For information, I use to work with catchments of size 1-10 km2 with 2-3 Mio elements (mesh size 5 m or less). I think larger elements would still work fine with FV though.

Please give feedback here!

Good luck,
PL

now i modified the pluie example cas. file with finite volume
telemac2d stop with an error but tidal flats opion is activated




PROSOU : TIDAL FLATS OPTION MUST BE ACTIVATED
WITH SCS CN RUNOFF MODEL

PLANTE: PROGRAM STOPPED AFTER AN ERROR
RETURNING EXIT CODE: 2



/

---

/ TELEMAC2D Version v7p2
/ VALIDATION TEST FOR RAIN IN 2D- here option 2:
/ 1- case without infiltration
/ 2- case with CN rainfall-runoff model and CN values in formatted
/ data file
/ 3- case with CN rainfall-runoff model and CN values in geometry
/ file and rainfall defined as a hyetograph in formatted data file
/
/ Statistics of CPU Time
/
/ Lenovo D30 2.8 MHz Nag compil.(1procs): 2s version 7.2 20/08/16
/ Lenovo D30 2.8 MHz Nag compil.(8procs): <1s version 7.2 20/08/16
/
/

---

RAINFALL-RUNOFF MODEL = 1
DURATION OF RAIN OR EVAPORATION IN HOURS = 6.
ANTECEDENT MOISTURE CONDITIONS = 2
OPTION FOR INITIAL ABSTRACTION RATIO = 1
RAIN OR EVAPORATION = YES
RAIN OR EVAPORATION IN MM PER DAY = 100.0
NUMBER OF PRIVATE ARRAYS = 3
FORMATTED DATA FILE 2 =runoff_data.dat
/
/

---

/ EQUATIONS
/

---

FRICTION COEFFICIENT =70
LAW OF BOTTOM FRICTION =3
VELOCITY DIFFUSIVITY =1.E-6
TURBULENCE MODEL =1

/

---

/ EQUATIONS, BOUNDARY CONDITIONS
/

---

/PRESCRIBED FLOWRATES =0
/PRESCRIBED ELEVATIONS =0
/VELOCITY PROFILES =1;4
/OPTION FOR LIQUID BOUNDARIES =1;1

/

---

/ EQUATIONS, INITIAL CONDITIONS
/

---

INITIAL CONDITIONS ='CONSTANT ELEVATION'
INITIAL ELEVATION =0.0
/

---

/ INPUT-OUTPUT, FILES
/

---

BOUNDARY CONDITIONS FILE ='t2d_geo_pluie.cli'
GEOMETRY FILE ='t2d_geo_pluie.slf'
RESULTS FILE ='res_rain_CN.slf'
FORTRAN FILE ='t2d_pluie_cn.f'
/ Fortran file used to print rainfall parameters to result file
/ (variables N,O,R), but the case works also without
/

---

/ INPUT-OUTPUT, GRAPHICS AND LISTING
/

---

LISTING PRINTOUT PERIOD =18
INFORMATION ABOUT SOLVER =YES
GRAPHIC PRINTOUT PERIOD =36
VARIABLES FOR GRAPHIC PRINTOUTS =U,V,B,H,S,L,F,N,O,R
MASS-BALANCE =true
/

---

/ INPUT-OUTPUT, INFORMATION
/

---

VALIDATION =NO
TITLE ='Test Rain'
/

---

/ NUMERICAL PARAMETERS
/

---

TREATMENT OF NEGATIVE DEPTHS =2
FREE SURFACE GRADIENT COMPATIBILITY =0.9
DISCRETIZATIONS IN SPACE =11;11
MATRIX STORAGE =3
SUPG OPTION =0;0
TYPE OF ADVECTION =1;5
CONTINUITY CORRECTION =YES
TREATMENT OF THE LINEAR SYSTEM =2
TIME STEP =200
TIDAL FLATS =YES
DURATION =28800
/

---

/ NUMERICAL PARAMETERS, SOLVER
/

---

SOLVER =1
SOLVER ACCURACY =1.E-6
MAXIMUM NUMBER OF ITERATIONS FOR SOLVER =2000
/

---

/ NUMERICAL PARAMETERS, VELOCITY-CELERITY-HIGHT
/

---

H CLIPPING =NO
IMPLICITATION FOR DEPTH =1.
IMPLICITATION FOR VELOCITY =1.
MASS-LUMPING ON H =1.
/
EQUATIONS = 'SAINT-VENANT VF'
FINITE VOLUME SCHEME = 5
VARIABLE TIME-STEP = YES
DESIRED COURANT NUMBER = 0.8
&FIN

Hi,

As I mentionned, you need to upgrade to version 7.3 to use FV as there are some bugs in 7.2...

Good luck!
PL

i made an update V7.3

now I must make a closed mash. "LORS DE L APPEL A CLOSE_MESH"

.....

NO SPECIFIC TREATMENT OF DRY ZONES
IN FINITE VOLUMES

EXITING LECDON. NAME OF THE STUDY:
Igensdorf 180min Rain

OPENING FILES FOR TELEMAC2D

*****************************
* MEMORY ORGANIZATION *
*****************************

ERREUR 1003 LORS DE L APPEL A CLOSE_MESH:GET_SRF_OBJ
TEXTE DE L'ERROR : HERMES_FILE_NOT_OPENED_ERR

PLANTE: PROGRAM STOPPED AFTER AN ERROR
RETURNING EXIT CODE: 2

short info:

after I have the version 8.0 installed, the finite volume calculation runs .... I estimate that I will instll on my computer soon to parallel on a linux system.

so i must learn linux

Thanks for the tips. I will contact you again if I have useful results.