Welcome, Guest
Username: Password: Remember me
Forgot your password? Forgot your username? Create an account
Forum
System Modules
TELEMAC-2D
Initial Conditions and Liquid Boundaries
Flat Threaded
  • Page:
  • 1
  • 2

TOPIC: Initial Conditions and Liquid Boundaries

Initial Conditions and Liquid Boundaries 6 years 3 months ago #31045

  • dh48
  • dh48's Avatar
Hi,

I am having trouble with my initial conditions on one of my inflow boundaries (Boundary 2; left-hand side of mesh). When I run the simulation, I receive the following error:

ITERATION        0    TIME:   0.0000 S
 THE LIQUID BOUNDARIES FILE CONTAINS
           2  LINES WITH:
 Q(1)     Q(2)
 USING STREAMLINE VERSION 7.0 FOR CHARACTERISTICS
 GRACJG (BIEF) : EXCEEDING MAXIMUM ITERATIONS:      50 RELATIVE PRECISION:   0.3955939E-08
 GRACJG (BIEF) : EXCEEDING MAXIMUM ITERATIONS:      50 RELATIVE PRECISION:   0.7382774E-01
 GRACJG (BIEF) : EXCEEDING MAXIMUM ITERATIONS:      50 RELATIVE PRECISION:   0.4139544E-03
 GRACJG (BIEF) : EXCEEDING MAXIMUM ITERATIONS:      50 RELATIVE PRECISION:    1.072483
 GRACJG (BIEF) : EXCEEDING MAXIMUM ITERATIONS:      50 RELATIVE PRECISION:   0.1095959E-01
 GRACJG (BIEF) : EXCEEDING MAXIMUM ITERATIONS:      50 RELATIVE PRECISION:    1.146892
 GRACJG (BIEF) : EXCEEDING MAXIMUM ITERATIONS:      50 RELATIVE PRECISION:   0.3217670
 GRACJG (BIEF) : EXCEEDING MAXIMUM ITERATIONS:      50 RELATIVE PRECISION:   0.1387811E-01
 GRACJG (BIEF) : EXCEEDING MAXIMUM ITERATIONS:      50 RELATIVE PRECISION:   0.4500793E-02
 DEBIMP: PROBLEM ON BOUNDARY NUMBER      2
         GIVE A VELOCITY PROFILE
         IN THE BOUNDARY CONDITIONS FILE
         OR CHECK THE WATER DEPTHS.
         OTHER POSSIBLE CAUSE:
         SUPERCRITICAL ENTRY WITH FREE DEPTH
         IN THIS CASE GIVE A POSITIVE DEPTH
         IN THE INITIAL CONDITIONS
         OR PRESCRIBE THE DEPTH AT THE ENTRANCE.

 PLANTE: PROGRAM STOPPED AFTER AN ERROR

I am aware that the 'supercritical entry' error indicates that there is no water on the boundary, meaning that TELEMAC can't compute a result. I have experimented with different values for PRESCRIBED ELEVATIONS and INITIAL ELEVATION, however i receive the same error.

I have also tried experimenting the Velocity Profiles on Boundary 2, all of which give the same error except from OPTION 1, which tends to get stuck after 2 iterations. I have also tried initialising using 'ZERO DEPTH' or 'CONSTANT DEPTH'/'INITIAL DEPTH' however receive the same error or it gets stuck after a few lines of the following:

GRACJG (BIEF) : EXCEEDING MAXIMUM ITERATIONS:      50 RELATIVE PRECISION:   0.4500793E-02

I obviously haven't got a full grasp of the initial conditions and i'm hoping someone can help me along with this.

See model files attached.

Thanks in Advance!


File Attachment:

File Name: riverdon.cas
File Size: 4 KB


File Attachment:

File Name: inverurie_2018-07-28-2.cli
File Size: 32 KB
The administrator has disabled public write access.

Initial Conditions and Liquid Boundaries 6 years 3 months ago #31050

  • riadh
  • riadh's Avatar
Hello

Before focusing on the boundary, remark that your solver is not converging (exceeding maximum number of iterations ). Which is probably caused by a big time step (5s with a cold start) and a very strict solver accuracy (10-14).

Please start by :
1- decrease your time step gradually
2- set solver accuracy to 10-6 for instance
3- use velocity profile 4 instead of 5
4- set real values to keyworkds asking for double precision (duration, time step, prescribed elevation, etc.) i.e. set TIME-STEP=1. for instance
5- cold start is always hard to converge, what you can do to smooth it, is to increase the prescribed discharge gradually (using liquid boundary conditions)

I hope this helps

with my best regards

Riadh
The administrator has disabled public write access.

Initial Conditions and Liquid Boundaries 6 years 3 months ago #31060

  • dh48
  • dh48's Avatar
Hi Riadh,

Thanks for getting back to me! I have taken your advice an adjusted my case file to reflect your suggestions. I have fixed my initial/boundary conditions and the model is now running successfully. However I still exceed maximum iterations for K-epsilon step and at 'BALANCE OF WATER VOLUME' at each time step (see below) so i think the model is still struggling to converge.

DIFFUSION-PROPAGATION STEP
 CVTRVF_POS_2 (SCHEME 13 OR 14):  10 ITERATIONS
 GRACJG (BIEF) :        2 ITERATIONS, RELATIVE PRECISION:   0.5919490E-06
 POSITIVE DEPTHS OBTAINED IN    10 ITERATIONS
--------------------------------------------------------------------------------
                          K-EPSILON MODEL
 GRACJG (BIEF) : EXCEEDING MAXIMUM ITERATIONS:      50 RELATIVE PRECISION:   0.4534494E+12
 GRACJG (BIEF) : EXCEEDING MAXIMUM ITERATIONS:      50 RELATIVE PRECISION:   0.2502503E+16
--------------------------------------------------------------------------------
                       BALANCE OF WATER VOLUME
     VOLUME IN THE DOMAIN :   0.2258763E+08 M3
     FLUX BOUNDARY    1:    -1701.324     M3/S  ( >0 : ENTERING  <0 : EXITING )
     FLUX BOUNDARY    2:     30.00000     M3/S  ( >0 : ENTERING  <0 : EXITING )
     FLUX BOUNDARY    3:     257.7800     M3/S  ( >0 : ENTERING  <0 : EXITING )
     RELATIVE ERROR IN VOLUME AT T =        85.50     S :   -0.4223155E-13
 GRACJG (BIEF) : EXCEEDING MAXIMUM ITERATIONS:      50 RELATIVE PRECISION:   0.1234383E+23
 GRACJG (BIEF) : EXCEEDING MAXIMUM ITERATIONS:      50 RELATIVE PRECISION:   0.2691550E+26
 GRACJG (BIEF) : EXCEEDING MAXIMUM ITERATIONS:      50 RELATIVE PRECISION:   0.2155615E+34
 GRACJG (BIEF) : EXCEEDING MAXIMUM ITERATIONS:      50 RELATIVE PRECISION:   0.5123180E+26
 GRACJG (BIEF) : EXCEEDING MAXIMUM ITERATIONS:      50 RELATIVE PRECISION:   0.4847854E+28
 GRACJG (BIEF) : EXCEEDING MAXIMUM ITERATIONS:      50 RELATIVE PRECISION:   0.1956511E+35
 GRACJG (BIEF) : EXCEEDING MAXIMUM ITERATIONS:      50 RELATIVE PRECISION:   0.1358362E+43
 GRACJG (BIEF) : EXCEEDING MAXIMUM ITERATIONS:      50 RELATIVE PRECISION:   0.9182931E+33
 GRACJG (BIEF) : EXCEEDING MAXIMUM ITERATIONS:      50 RELATIVE PRECISION:   0.1015167E+45
 GRACJG (BIEF) : EXCEEDING MAXIMUM ITERATIONS:      50 RELATIVE PRECISION:   0.2482935E+37
 GRACJG (BIEF) : EXCEEDING MAXIMUM ITERATIONS:      50 RELATIVE PRECISION:   0.3369457E+47
 GRACJG (BIEF) : EXCEEDING MAXIMUM ITERATIONS:      50 RELATIVE PRECISION:   0.1039895E+45

Can you provide further insights on how to resolve this? I see you mention a 'cold start' and to increase the discharge gradually using .liq boundaries. Does this involve increasing the discharge until convergence, and then using these results as a hot start for my actual flood event simulation? (my discharge values are from a hydrograph for 1 in 100) event.

Could my model be struggling to converge due to mesh quality also? I will try attach my .slf file to show you my mesh (i tried last time but file was too big). I think some of my elements are bit skewed due to the meandering angle of the river. Can you make any suggestions on how to refine my mesh?

Kind Regards,

David
The administrator has disabled public write access.

Initial Conditions and Liquid Boundaries 6 years 3 months ago #31087

  • riadh
  • riadh's Avatar
Hello David

To fix he problem with K-eps, you have to increase the maximum of iterations for the solver of K-eps. You have to use the following keyword:
MAXIMUM NUMBER OF ITERATIONS FOR K AND EPSILON= 500
For your case, you do not even need to use k-eps model, you can use simply constant viscosity (TURBULENCE MODEL=1 and VELOCITY DIFFUSIVITY=0.1)

As you mentioned also, try to keep an acceptable quality for the mesh.

I hope this helps.
with my best regards

Riadh
The administrator has disabled public write access.

Initial Conditions and Liquid Boundaries 6 years 3 months ago #31094

  • dh48
  • dh48's Avatar
Hi Riadh,

I have made these amendments to my case file and managed to refine my mesh. My model now seems to be converging and is running a lot smoother, thanks for your help!

Best Wishes,

David
The administrator has disabled public write access.

Initial Conditions and Liquid Boundaries 5 years 10 months ago #32367

  • greeshmaranjith1
  • greeshmaranjith1's Avatar
i am trying to make simulation with imposing hydrograph at two boundaries and two boundaries with tide (TPXO) but i am getting following error. can anyone help? i am very to telemac.
Attachments:
The administrator has disabled public write access.

Initial Conditions and Liquid Boundaries 5 years 10 months ago #32369

  • riadh
  • riadh's Avatar
Hello

this means that you boundary is getting dry.
first, run the model without hydrograph and then introduce these latter.
reduce time step value also;

kind regards

Riadh
The administrator has disabled public write access.

Initial Conditions and Liquid Boundaries 5 years 10 months ago #32370

  • greeshmaranjith1
  • greeshmaranjith1's Avatar
sir,
i tried as you said. first simulation was run without imposing hydrograph for one day then using that result.slf file i tried to run with hydrograph but the following error is showing.
Attachments:
The administrator has disabled public write access.

Initial Conditions and Liquid Boundaries 5 years 10 months ago #32422

  • greeshmaranjith1
  • greeshmaranjith1's Avatar
i am still stuck with it. can anyone help?
The administrator has disabled public write access.

Initial Conditions and Liquid Boundaries 5 years 10 months ago #32425

  • riadh
  • riadh's Avatar
Hello

The error message is explicit. You are giving a latitude of a point which is not in degree (in the interval [-180,180]).
In you steering file you have

SPATIAL PROJECTION TYPE =3

which means that the coordinates in the geometry file are given in longitute/latitude. I think that this is not your case, since you are using seemingly cartesien coordinates. So change the value to 1 or 2 depending on your data.
Please read the manual for more details.

kind regards

Riadh
The administrator has disabled public write access.
Flat Threaded
  • Page:
  • 1
  • 2
Moderators: pham
Forum
System Modules
TELEMAC-2D
Initial Conditions and Liquid Boundaries

The open TELEMAC-MASCARET template for Joomla!2.5, the HTML 4 version.