open TELEMAC-MASCARET The mathematically superior suite of solvers

Hello,

I made a computation with an unsteady hydrograph for discharge upstream and Stage-Discharge-Curve downstream. My RELATIVE ERROR CUMULATED ON VOLUME seems too high. Do you have an Idea if the Error is too high and what I can do to reduce the error?

I attached the cmd-END-Message, cas-file and geometry file.

Thank you very much!

Hello


You are using a non conservative scheme that makes roughly a relative error of about 10-6 that means that you loose roughly about 5m3 of water on each time step (over more the 57 millions of cubic meters in your domain). You simulated more than 27 days (more than 250 000 time steps), the balance is quickly obtained (and explained) :)

to obtain better mass conservation, use schemes 13 or 14 instead of scheme 1

with my best regards

Riadh ATA

Thanks for your reply :)

Hello,

You have a low accuracy of you linear solver :SOLVER ACCURACY =1.E-3, you can try 1.E-4 to 1.E-6, but there is another solution:

You still can have machine accuracy with the following keywords :

TIDAL FLATS : YES
OPTION FOR THE TREATMENT OF TIDAl FLATS : 1
TREATMENT OF NEGATIVE DEPTHS : 2
CONTINUITY CORRECTION : YES

This has the consequence that the continuity equation is redone with machine accuracy after the linear system.

With :

TREATMENT OF THE LINEAR SYSTEM : 2
SOLVER : 1

it will go much faster.

With best regards,

Jean-Michel Hervouet

Hello Jean-Michel Hervouet

Thanks for your answer. I tried it as you said but I got an error message. It is attached.

Maybe you can have a look?

Thank you very much!

Hello,

as the listing says, you must set in the steering file:
MASS-LUMPING ON H =1.0

Best regards,
Clemens

I have modified steering file as per your instruction for the error but still I getting same error

ADVECTION STEP

---

DIFFUSION-PROPAGATION STEP
GRACJG (BIEF) : 4 ITERATIONS, RELATIVE PRECISION: 0.5650409E-07
POSITIVE DEPTHS OBTAINED IN 10 ITERATIONS

---

BALANCE OF WATER VOLUME
VOLUME IN THE DOMAIN : 0.4491200E+08 M3
FLUX BOUNDARY 1: -439.6126 M3/S ( >0 : ENTERING <0 : EXITING )
RELATIVE ERROR IN VOLUME AT T = 0.4499E+05 S : 0.3112375E-14

================================================================================
ITERATION 4500 TIME: 12 H 30 MIN 0.0000 S ( 45000.0000 S)

---

ADVECTION STEP

---

DIFFUSION-PROPAGATION STEP
GRACJG (BIEF) : 4 ITERATIONS, RELATIVE PRECISION: 0.5956097E-07
POSITIVE DEPTHS OBTAINED IN 10 ITERATIONS

---

BALANCE OF WATER VOLUME
VOLUME IN THE DOMAIN : 0.4490760E+08 M3
FLUX BOUNDARY 1: -439.4086 M3/S ( >0 : ENTERING <0 : EXITING )
RELATIVE ERROR IN VOLUME AT T = 0.4500E+05 S : -0.1182212E-13

---

FINAL BALANCE OF WATER VOLUME

RELATIVE ERROR CUMULATED ON VOLUME: -0.6295246E-15

INITIAL VOLUME : 0.6012306E+10 M3
FINAL VOLUME : 0.4490760E+08 M3
VOLUME THAT ENTERED THE DOMAIN: -0.5967399E+10 M3 ( IF <0 EXIT )
TOTAL VOLUME LOST : -0.3784895E-05 M3

END OF TIME LOOP

CALL OF P_EXIT IN ITS VOID VERSION

CORRECT END OF RUN

ELAPSE TIME :
1 MINUTES
14 SECONDS


~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~

... handling result files

+> en.cas
moving: en_res_test_6.slf


My work is done

Hi,

which error do you mean?

In your listing output you have RELATIVE ERROR CUMULATED ON VOLUME: -0.6295246E-15, which is perfect.

Best regards,
Clemens