open TELEMAC-MASCARET The mathematically superior suite of solvers

Hello ,

i have used the following keywords and simulated the flow for a domain using telemac2d solver

ABSCISSAE OF SOURCES : 292024.43750000000
ORDINATES OF SOURCES : 2069284.1250000000
VELOCITIES OF THE SOURCES ALONG X : 0.1
VELOCITIES OF THE SOURCES ALONG Y : 2.12
WATER DISCHARGE OF SOURCES : 3.8

In the result file, the velocities stored at that source point are not showing as per the inputs (VELOCITIES OF THE SOURCES ALONG X & VELOCITIES OF THE SOURCES ALONG Y).

Why is this happening?


Thanks
Sathya

Hi,

WATER DISCHARGE is a volume of water added in the domain, generating velocities in every direction (as you can see if you set VELOCITIES OF THE SOURCES ALONG X/Y = 0)
whereas
VELOCITIES OF THE SOURCES are a momentum flux added to the fluid potentially already in motion (it can be shown as a relative velocity: (U_source-U_fluid)*DISCHARGE/AREA/H). So the discharge you are prescribing also affect the velocities in the domain and it's rather normal that your computed velocities are not equal to the prescribed velocities of the source because of the velocities generating by the discharge.


To sum-up, and if I'm not mistaken, velocities of the sources are used to forced the discharge to flow in the suited direction. But the water mass injected in the domain is control by the water discharge.

I hope it helps.

Regards,
Laurent

Hi,
Thanks for the explanation.

In the above statement, you have given

relative velocity = (U_source-U_fluid)*DISCHARGE/AREA/H)

I would like to know what is AREA?
Is it area of elements surrounding the point source node?
or
Area of single element where the point source located?

Thanks
Sathya

Hi,

The statement given is not homogeneous to a velocity, it's the source term added to the momentum equation in prosou.f.
This is the area surrounding the point(s) where the source is applied.

Regards,
Laurent

Hi,
Thanks for your clear information.

I have a question though.

Suppose if i need to get exactly the prescribed velocities at the source point (node), what should i do to achieve it?

Thanks

Hi,

As said in the other post and in the user manual, if you want to prescribe the discharge by means of the velocities, you have to use in your steering file:
- a SOURCE REGIONS DATA FILE (polygon delimiting your source point(s)),
- the VELOCITIES OF THE SOURCES ALONG X/Y (not the WATER DISCHARGE OF SOURCES)
- the attached modified subroutine telemac2d.F (small bug at line 884)



With this settings, the discharge will be prescribed as the norm of your velocity times the area where you prescribe it (that is different than with WATER DISCHARGE OF SOURCES).

Be aware that according to your mesh resolution near the sources and the values you want to prescribe, the velocities can be + or - impacted by the discharge, and it is possible that you will not have exactly the same values. Your mesh may need to be adapted.

Note that the velocities are also affected by other processes you consider in your modelling (wind, friction...).

I hope it helps.

Regards,
Laurent

PS: In case you want to prescribe exactly both discharge and velocities, I'm not sure it is possible (over-constrained system).