open TELEMAC-MASCARET The mathematically superior suite of solvers

Hello,

Can anyone advise the best way to introduce a submerge sea water intake (2meter high and 5meter width, and 2 meter above the bottom for example)with a fixed flowrate into telemac3d?

Thanks in advance.

Mathieu

Hi

You could use the sources point but without any control of the intake section.
You could also create an island in your model and gives a vertical profile at the boundary condition;

Regards

Thanks for the quick answer, I will try the 2nd suggestion at first.

Hello,

I have try to implement a vertical profile at the boundary condition. But it looks that Telemac-3d is not taking my vertical profile into consideration.

I will explain my problem again, I use a PRESCRIBED FLOWRATES at the 3rd boundary of my model, and I wish to have the flowrates only at the 2nd layer (5 layers total)all along the 3rd boundary.

Could you explain me with more details on how I can do that? A template would be awesome.

Thanks and regards,

Mathieu

Hello,

Here is the basic procedure :

Use the key-word "VELOCITY VERTICAL PROFILE" (one integer per boundary. For the 3rd boundary you must have a 0 to say that the profile is user defined. Then you must put the function VEL_PROF_Z in your FORTRAN FILE and implement the part IOPT=0 (in your case you just put VEL_PROF_Z=0.D0 or VEL_PROF_Z=1.D0 depending on the plane number IPLAN.

With best regards,

Jean-Michel Hervouet

I already try to modified the vel_prof_z.f but I haven't the expected result.
I kept the logarithmic profile and I add the following line :

IF(IPOIN2.EQ.1086.AND.IPLAN.EQ.1)THEN
VEL_PROF_Z=0.D0
ENDIF
IF(IPOIN2.EQ.1086.AND.IPLAN.EQ.2) THEN
VEL_PROF_Z=0.D0
ENDIF
IF(IPOIN2.EQ.1086.AND.IPLAN.EQ.3) THEN
VEL_PROF_Z=1.D0
ENDIF
IF(IPOIN2.EQ.1086.AND.IPLAN.EQ.4) THEN
VEL_PROF_Z=0.D0
ENDIF
IF(IPOIN2.EQ.1086.AND.IPLAN.EQ.5) THEN
VEL_PROF_Z=0.D0
ENDIF

(The boundary condition is made of 3 horizontale nodes and 5 layers and a prescibed flowrates).

Is it the good way to proceed, cause I can see any difference when I am checking the vectors at the node 1086 (at the 5 layers)?

Thanks in advance.

Hello,

Well this seems OK. If you insert the subroutine BORD3D.F in your Fortran file you can see where the function vel_prof_z is called and check what gets out. You can also check in the function if IPOIN2=1086 happens, by adding a flag in your implementation.

Now check also that 1086 is the global number of your point in the numbering of all points of the mesh, not the numbering of the boundary points. Furthermore in parallel it will not work, in that case you should do the test on : MESH2D%KNOLG%I(IPOIN2).

Let's see if one of these hints is the right one...

Jean-Michel Hervouet

Thanks a lot for your help, I finally made the vertical velocity profil work.

The only remaining problem is that I have to change the value of VERPROVEL into the fortran code so the code execute the VEL_PROF_Z fonction (see below)(I put VELOCITY VERTICAL PROFILES=0 in the cas file):

VERPROVEL(IFRLIQ)=0
IF(VERPROVEL(IFRLIQ).NE.1) THEN
WRITE(*,*) 'lteq1'
PROFZ=VEL_PROF_Z(IFRLIQ,NBOR2%I(K),
* AT,LT,NP,INFOGR,VERPROVEL(IFRLIQ))
UBORL%R(IJK) = UBORL%R(IJK)*PROFZ
VBORL%R(IJK) = VBORL%R(IJK)*PROFZ

ENDIF

Do you have any idea why I have this problem?

Thanks again and regard,

Mathieu

Hello,

As you want this profile on the 3rd boundary, you must have :

VELOCITY VERTICAl PROFILES = 1;1;0

so that 0 is meant for boundary 3. Is that the problem ?

With best regards,

Jean-Michel Hervouet

Hello,

Many thanks for the help, everything is working perfectly now.

Best regards,

Mathieu