open TELEMAC-MASCARET The mathematically superior suite of solvers

Good afternoon everyone,

I am using a Telemac2D model with weirs and noticed that, at certain timesteps, although the normal velocity on the weir nodes is zero and the corresponding conditions are applied (variables LIHBOR, LIUBOR and LIVBOR equal 2), the resulting normal velocity on the boundary is not zero. The boundary conditions seem to be modified after the call to CLSING. Which subroutine could override the variables mentioned above?

Many thanks in advance,

C.C.

PS : I am using Thompson boundary conditions. I also checked that CLHUVT imposes correct values for the LIHBOR, LIUBOR and LIVBOR variables.

Hello,

Actually the formulas giving the velocities on both sides of the weir do not exactly ensure that the discharge will be the same (this is due to discretisation of the discharge as the product of two linear functions), so an average is done in subroutine propag. However if velocities are zero on both sides this should not change anything, so I am not sure that this will explain your remark. Another point is Thompson boundary conditions, this should not be applied to the weir, I assume that Thompson is for another boundary ?

Regards,

JMH

Thank you Jean-Michel,

You are right indeed about the Thompson condition: it is only applied on another boundary.

After digging further, it seems that, after the call to PROPAG, the velocity is not zero (not even tangential), even though the variables UBOR and VBOR have the correct values (0.0 in this case).

=> What could prevent the correct transmission of the UBOR/VBOR values into the final U/V variables?

Hello,

I looked more precisely at this problem. In fact the boundary conditions are treated in propag.g at line 1619 (case of wave equation). If we have a prescribed value (LIUBOR=6 for example) this value will be put there. If we have no flow (LIUBOR=2 as you say) then nothing is done and the boundary is treated like other walls, i.e. we have a weak treatment, which means that the flux taken into account in the continuity will be 0, but the velocity is let free. This is the weak way of imposing u.n = 0. So you may see a normal component of velocity (that should remain small however, it should tend to 0 if the mesh size tends to 0 and gives you an idea of the finite element approximation error at that place), but even with that normal component no flux is considered.

So your remark is valid also for any solid boundary.

With best regards,

Jean-Michel Hervouet