open TELEMAC-MASCARET The mathematically superior suite of solvers

Hi, I need to impose a boundary condition for BED LOAD as a time-series of DISCHARGE INFLOW. The SISYPHE´s manual said: you have to create a LIQUID BOUNDARY FILE and the SISYPHE´s boundary condition file (.cli) must contain the flags as shown below:

4 5 5 0.0 0.0 0.0 0.0 4 0.0 0.0 0.0 565 1

Then you have to included the keyword PRESCRIBED SOLID DISCHARGES with an arbitrary value.

... I did all this, but there was an error:


FIRST VALUE MUST BE TIME_RFC, DENOTED TSTOP 1

IN FILE OF LIQUID BOUNDARIES

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


My liquid boundary file is (in steering file sisyphe):

T Q2BOR(2)
s m3/s
0 0.003819261
1330 0.003819261
2173 0.099210236
2842 0.178578426
3344 0.198420473
4682 0.128973307
5518 0.093257622
6354 0.065478756
7190 0.043652504
8026 0.025794661
8862 0.013889433
9699 0.001152606
10360 0.003819261

I don´t understand why it doesn´t work. So I need your help to fix that.

1) I need another things to do or correct any file ?
2) LIQUID BOUNDARY FILE have to be in sis.cas (without other variables) or t2d.cas (with other variables) ?
3) Unit BED-LOAD sediment is really m3/s or m2/s?
4) Name of variable BED-LOAD sediment is really Q2BOR or QBOR


Best regards..

Hi,

I have the same question that the problem described above on the post .
I understand how to fix the boundary and the keyword PRESCRIBED SOLID DISCHARGES.
However, I would like to make the solid inflow unsteady:
- or with a transport rate function of the liquid inflow (or the depth) in m2/s
- or with a solid flow in m3/s

How should I set up? What is the format of the liquid file?

Thank in advance for your answer.

Bests regards

Hi,

I used the next LIQUID BOUNDARY FILE (in sisyphe .cas):

T Q2BOR(2)
s m2/s
0 0.1
3600 0.2
7200 0.3

...but there was an error:

================================================================================
Q2BOR(2)

QG: MORE PRESCRIBED SOLID DISCHARGES
ARE REQUIRED IN THE PARAMETER FILE
AT LEAST 2 MUST BE GIVEN

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

Then, I changed Q2BOR(2) by QG(2) as error said.
Now the program works, but it does not take the values assigned in the LIQUID BOUNDARY FILE for BED-LOAD FLUX.

the listing printouts shows:

================================================================================
ITERATION 60 TIME: 1 MN 0.0000 S ( 60.0000 S)

MASS-BALANCE (IN VOLUME, INCLUDING VOID):
SUM OF THE EVOLUTIONS : -0.1084202E-18 M3
BOUNDARY 1 BEDLOAD FLUX = -0.000000 ( M3/S >0 = ENTERING )
BOUNDARY 2 BEDLOAD FLUX = -0.000000 ( M3/S >0 = ENTERING )
TOTAL BEDLOAD FLUX = -0.000000 ( M3/S >0 = ENTERING )
LOST VOLUME : -0.1084202E-18 M3 ( IF <0 EXIT )

MAXIMAL EVOLUTION : 0.9876476E-06 NODE : 35743
MINIMAL EVOLUTION : -0.2136524E-05 NODE : 35744
TOTAL MAXIMAL EVOLUTION : 0.5099936E-04 NODE : 35743
TOTAL MINIMAL EVOLUTION : -0.1107080E-03 NODE : 35744
MAXIMUM COURANT NUMBER: 0.5262998E-01
TIME-STEP : 1.000000

================================================================================

2 BEDLOAD FLUX shouln´t be 0. Does anyone know why? QG is equal to Q2BOR ?? and whats units should have ?

Hi,

I managed to run a simulation with Liquid Boundary File for Sisyphe (version V8P0)
As you did, it's necessary to put QG instead of Q2BOR. Remenber that the unit is m3/s (without porosity).

Moreover you have to put a value in conlim for the Q2BOR for each point of the boundary. It give the profil of solid inflow. For example, I put 4 5 5 1 0 0..4... in each point of my boundary for a constant profil (the example in the part "time-serie of sediment discharge" in the chapter 2.7.2 of the manual is wrong because it shows a 0 for Q2BOR)

You can see how it works in the subroutine DISIMP.f.

I hope it helps you.
If not, give me your files to compare with the mines.

Best regards

Thanks for your response.

In the conlim example that you give:

4 5 5 1 0 0..4...

That 1 is =Q2BOR (m2/s) rigth ??

I ran my simulation ass you said with a next LIQUID BOUNDARY FILE:

========================================================================
T QG(2)
s m3/s
0 1.14
60 2.28
120 3.42
180 4.56
240 5.7
300 6.84
360 7.98
420 9.12
480 10.26
540 11.4
600 12.54
========================================================================

and the next BOUNDARY CONDITION FILE (only inflow liquid boundary):

=======================================================================
4 5 5 0.01 0.000 0.000 0.000 4 0.000 0.000 0.000 744 362
4 5 5 0.01 0.000 0.000 0.000 4 0.000 0.000 0.000 757 363
4 5 5 0.01 0.000 0.000 0.000 4 0.000 0.000 0.000 766 364
4 5 5 0.01 0.000 0.000 0.000 4 0.000 0.000 0.000 776 365
4 5 5 0.01 0.000 0.000 0.000 4 0.000 0.000 0.000 782 366
4 5 5 0.01 0.000 0.000 0.000 4 0.000 0.000 0.000 790 367
4 5 5 0.01 0.000 0.000 0.000 4 0.000 0.000 0.000 794 368
=======================================================================

If I unsderstand you: My profile measure B=114 (m) so, at time T=0 (s) it should be QG=Q2BOR*B => 1.14= 0.01 * 114. But, what happen at the time T>0 ? The results shows that bed-load flux is 1.14 (m3/s) in every time in simulation. It seens that not take the thers values of time. Even if I changed values of LIQUID BOUNDARY FILE, the program keeps the same value =0.01 by conlim (BOUNDARY CONDITION FILE). I don´t know how you did to take all time-serie for discharge, because the value 0.01 in conlim is constant (for all time).

Any other suggestion?

Best regards.

Do you see the values from your liquid boundary file in the listing?
For simulation times > 0 it should interpolate between 2 values and I think these values are listed in the listing. If not the reason could be that the program doesn't read or take your liquid boundary file.

I would firstly try to run without liquid boundary file but with the PRESCRIBED SOLID DISCHARGES = 0;1.14 given in the cas-file. If that is working I would try again the liquid boundary file. The keyword should be there even if you have the liquid boundary file.

Instead of 0.01 in the conlim file I would use 1. If the value is the same for the whole inflow boundary the solid discharge is distributed uniform at the inlet.
You give the solid discharge in m3/s either in the cas-file or in the liquid boundary file and that is calculated with the corresponding length and a weighting factor (4th line conlim) for one boundary node from sisyphe to a qsbor in m2/s for that boundary node.

Sometimes we have problems with ascii files due to linux/windows different end of lines etc. You can choose the right format in an editor. Additionally no comments are allowed in 2 following lines of the liquid boundary file. So pay attention to these two lines.
T QG(2)
s m3/s

Best regards

Thanks for your reply. Now it works. :)

Hi,

I think that the value of Q2BOR in the conlim file is just the shape of the distribution or repartition (the profil). The value doesn't matter but have to be different from 0. It's the same for the keyword PRESCRIBE SOLID DISCHARGE in the steering file, you have to put it but Sisyphe don't take it into account. It's only the value of the liq file for Sisyphe that is important.

I give you my configuration:

SISYPHE STEERING FILE:
PRESCRIBED SOLID DISCHARGE = 0.01;0

CONLIM OF SISYPHE
4 5 5 0.01 0.0 0.0 0.0 4 0.0 0.0 0.0 196253 476
4 5 5 0.01 0.0 0.0 0.0 4 0.0 0.0 0.0 196258 477
4 5 5 0.01 0.0 0.0 0.0 4 0.0 0.0 0.0 196261 478
4 5 5 0.01 0.0 0.0 0.0 4 0.0 0.0 0.0 196265 479
.....

LIQ OF SISYPHE:
T QG(1)
s m3/s
0 1
8000 10

My first timestep:
BOUNDARY 1 BEDLOAD FLUX = 1.685417 ( M3/S >0 = ENTERING )

My last time step:
BOUNDARY 1 BEDLOAD FLUX = 16.66667 ( M3/S >0 = ENTERING )


The difference of values between my liq file and the bedload flux in the listing is normal because the discharge in the liq file is without the porosity althought the listing take it into account (see the note at the bottom of page 26 of the manual).

Hope it helps you

Regards

Antonin wrote:
Hello Antonin

Does this work only with V8P0 ? I'm having the same issues Gustavo had (sisyphe using PRESCRIBE SOLID DISCHARGE and not loading values from the *.liq file with QG(t)) and I'm using V7p1.

Thanks

Best regards

Hi,

I've just tried my test modele with the V7P1 version of Telemac and the solid discharge is equal to the PRESCRIBE SOLID DISCHARGE. The liq file seems not to be considered.

I advice you to install the V8P0.

Regards