open TELEMAC-MASCARET The mathematically superior suite of solvers

Hi,

I'm making some test with BlueKenue. I can't figure out how to extract a flow, in m3/s. It's easy for velocity or water depth but not for flow.

For example, in my model, there's an island. I want to know the flow going on the left of this island.

If BK doesn't have this feature, does Ruben have it ? If yes (lots of "if" ...), where do i get Rubens, i don't have it with my SVN repository v6p1 version of telemac2d.


Thanks.

Hi Alex,

This is functionality that I have wanted to consolidate into a simple tool for a while but unfortunately haven't had the time.

So in the meantime here is the procedure...

1. The simulation result file should have the two variables VELOCITY UV and DEPTH. If depth is not there, calculate it with the calculator as: free surface minus bottom.

2. Compute Flux in U using "Tools->Calculator". Multiply Component U of VELOCITY UV by DEPTH. Store it UH (do for all time steps)

3. Compute Flux in V using "Tools->Calculator". Multiply Component V of VELOCITY UV by DEPTH. Store it VH (do for all time steps)

4. In the Workspace select the UH object.

5. Using "Tools->Create Vector Field" generate a flux vector object. Select VH as the V component and make sure that the "All Frames" option is turned on. Default new object name is "UH+VH.t3v"

6. Using the "new Open Line" button create your section.

7. Click on "View->T3 Mesh Toolbar"

8. Make sure this newOpenLine is selected in the WorkSpace and select the "Integral button" on the "T3 Mesh Toolbar".

9. When the Integration Dialog comes up Select the UH+VH object as the Gridded data to be integrated. Provide a name and units for the resulting time-series and click OK.

And you're done...

Cheers... Martin

A little bit of additional information...

You can have multiple lines (sections) in the lineset. A separate timeseries is generated for each line.

Cheers... Martin

Thanks for the clear answer.

I've tested it on the "wesel" example. It's quite easy and fast to do.

The result is something oscillating in time between 1100 and 1150 m3/s. Im' not sure where do the oscillation (in time) comes from but it's no big deal.

However I can't link it to the input flowrate, witch is suppose to be 1061.
First how can't it be exactly the same ? There are no "reservoir effect" on this wesel model.

Second, in the curve editor under FUDAA, the flow rate is supposed to bet in m2/s. If i multiply this by the length of the boundary condition (420 m), the flow is going to be ... 1061*420 = way to high.

What do i not understand ?

Hi Alex,

If you can afford to rerun your simulation and don't mind using a bit more disk space, you could save scalar flowrate (Q) to your slf result file. Add it to your GRAPHIC PRINTOUT line.

example:

VARIABLES FOR GRAPHIC PRINTOUT : U,V,H,B.....Q;

After you open your results in BlueKenue, you simply have to run steps 7 through 9 (see Martin's answer), but this time Integrate on the Scalar Flowrate layer directly.

This has been a time saver for me on several occasions. I've noticed a very slight difference between discharge calculated this way and what you get if you run steps 1-9 but that's probably due to discretization differences. In my case that difference is generally less than 0.5 %.

Regards,

jeremie

Thanks. It's faster indeed.

It seems that even if fudaa tells you that the flow rate is in m2/s, it is in fact in m3/s as we can see in the boundary condition file. That answer my first question.

Still, I have a different value of discharge between what is set in the boundary conditions file (1061 m3/s) and what I "mesure" with bluekenue (1100 to 1200 m3/s).

It's a 4% difference i can't explain.

Alex,

The differences are because Blue Kenue uses a linear interpolation of the values on an element. When computing these flows as a post-processing step there isn't enough information to do otherwise.

You can tell Telemac to compute the exact values during the simulation.

JMH (an/or others more knowledgeable than I) can provide more details.

Hope this answers your questions... Martin

Hi,

I've investigated some more on the differences between Martin's method and the use of the Q variable to integrate discharge across a section. It appears that the differences between both methods are very sensitive to the section's orientation. This is explained by the fact that Q is a scalar field whereas UH+VH is a vector field.

One can easily verify this by calculating discharge across a section parallel to the flow field. Integrating on UH+VH will more or less render a near 0 discharge, which is expected. However, integrating on Q will return a non-negligible discharge since the operation is performed on velocity magnitude without regard to orientation. This will lead to erroneous discharges if the section is not perfectly perpendicular to the flow field.

Instead of using Q, I recommend saving variables I,J which are the x and y components of scalar discharge. These will readily show up in BlueKenue as a vector field XY and can be integrated, as is, along a line. Integrating on a manually created UH+VH field will render identical results (within a 10E-6 margin).

Best regards,

jeremie