open TELEMAC-MASCARET The mathematically superior suite of solvers

Hi, there.

When I use telemac2d in some case to simulation pollutant profile, I met a problem as follows:

VTRVF: 200 SUB-ITERATIONS REQUIRED FOR THE
VF SCHEME. DECREASE THE TIME-STEP

The original time step I used is 5s,So I decreased it to 0.5s,even to 0.05s.

But the error kept occuring. Then I change the NITMAX to 300. It still doesn't work.

Could someone tell me the reason for the problem？

Another question is that I didn't set the scheme to VF SCHEME. What scheme is it? Is it default value? And what's the corresponding keyword for it?

Thanks in advance.

Best wishes

Hello,

This is generally due to a very high velocity or a tidal flat. In this latter case the advection to choose for tracers should be 13 or 14 (the same in 2D, they are just different in 3D)

The keyword in 2D is :

TYPE OF ADVECTION : 1;5;14

This would give : characteristics for velocity (the 1) and N-scheme adapted to tidal flats for tracer (the 14). The 5 in the middle refers to depth but is no longer used.

With best regards,

Jean-Michel Hervouet

Thank you for your reply, Jean-Michel.

But there is no tidal flat in my case.

And I run the case without tracer first, the velocity is not very high.

Can I change the scheme to avoid the problem?

Best wishes

Hello,

I would need to see your parameter file. You must ask for this advection scheme somewhere. Actually the message points out a large CFL, so you must have either zones with high velocities, or a very tiny element somewhere. You can try to have :

TYPE OF ADVECTION : 1;5;1;1

and see what happens, it will not be mass conservative for tracers but there will be no CFL limitation and you can have a result and see what happens.

With best regards,

Jean-Michel Hervouet

Thank you,Jean-Michel.

According to your suggestion, I found and correct some mistake.

But the same error occurs if I change 1;5;1 back to 1;5;4.

Would you please check the cas file for me?

Please see the attachment.

Hello,

I find no error in your parameter file, then try scheme 14 instead of 4 (if depth is very small somewhere), or look at your CFL number = velocity * (mesh size) / (time step), it must be 200 somewhere, which could be the case if you have an overlooked very small element.

JMH

Hello,

Also try :

IMPLICITATION FOR DEPTH = 1.

and/or

IMPLICITATION FOR VELOCITY = 1.

to have a more stable scheme.

JMH

Thank you, Jean-Michel.

Both of the two ways you suggested work, and it seems that the first method leads to better results:)

I still have some questions to consult you.

1)when 1:5:14 is used, should the TIDAL FLATS be set yes or no?
In my case, it remains the default value,i.e. ''no'', but the mistake was corrected. I don't know why.

2)For the variable to be exported Q, why is its unit is m2/s,not m3/s?

Best wishes.

Hello,

For scheme 14 to work properly if there are tidal flats, you need to have :

TIDAL FLATS : YES
TREATMENT OF NEGATIVE DEPTHS : 2

Even if you have positive water everywhere it will give you a continuity at machine accuracy.

The discharge is m2/s because it is given for every point and it is only depth*velocity. Only the integral along a boundary will give m3/s.

Regards,

JMH

Sorry, I was wrong.

The default value for TIDAL FLATS is YES.

Now I see.

Thank you for all:)