open TELEMAC-MASCARET The mathematically superior suite of solvers

Hello

I saw a few topics about bridges but none really answered my questions.

I want to model the flood of a river with 6 bridges. each bridge has a different shape (square, circle, arch, random ..)
Each bridge can be pressurized or not depending on the flow.

My question is : how do you model bridges ?

I tried using the Tubes data file but you can't choose the shape of the bridge.
Is there another way to model bridges ?

If I use the tube data file, do I need to rise the elevation data of the cross section to the level of the road to block the cross section except for the tube ?

Thanks for your answers

Hello

The bridge option provided in Telemac give a simple way to setup cases where the brigde gets pressurized. At the bridge location, the overflow will be considered as a standard free surface way, whereas the flow going through the bridge is considered only by the contribution of the flowrate (negative at the upstream face and positive at the downstream side). This flowrate is approximated as a flow in a cylindrical duct with a negative pressure gradient (due to friction head losses (amont others)). The real shape of the bridge is not considered, but only the effective section.
The local flow around the bridge can not be reproduced in a fine way with these approximate solutions, you need more sophisticated tools to reproduce more physical behavior.
There are some empirical formula that corrects the water level a posteriori that takes into account for some usual bridge shapes. You can find them in Borda-Carnot formulas, for instance, in the US department of Transportation, Hydraulics of bridge waterways, Hydraulic design series

I hope that this helps

with my best regards

Riadh ATA

Thank you for your answer

If I understand correctly :
- I can't choose the shape of the bridge, only a cylindrical duct
- So I have to choose a cylindrical duct that has approximatly the same area as the real bridge would have ?

So I have some other questions :
- to do the cylindrical duct, do you use the Tubes data file ?
- Can you visualise or represent in a post precessor or somehow the duct ?
- Do you change the Z data at the location of the bridge ? What I mean is do you leave the altitude at the bed level and add the duct or do you rise the altitude to the level of the road and add the duct underneath ?

Thank you again for your answer
Best regards

Hello,

You misunderstood somehow what I have written. You can not choose the shape of the bridge, but, I didn't mean that the only possible shape is the cylindrical one. The cylindrical shape is only used to estimate the flow through the tube.

Hereafter answers to you questions:
- yes, use Tubes data file
- no you can not visualize the duct
- you will find the answer in the discription of the parameter given un the tube data file. You will see how the upstream and downstream bed levels is taken into account.

With my best regards

Riadh ATA

Sorry, my english is not perfect, I might misunderstand you.

thanks again


When you use the tube data files, is your tube square or cylindrical ?
because you enter the height and width of the tube which makes me think it's rectangular.

In the tube data file, I don't find how the upstream and downstream bed levels is taken into account....
I found z1 and z2 which are The elevation of Entry and Exit points. I think it means the elevation at the bottom of the tube. And if I don't change my bed level to the level of the road how can I define the height of the concrete between the top of the tube and the road ?
And how can I prevent the water from going and the right and left side of the tube if my bed section is 15m large for exemple and the tube only 10m large, the rest of the section being concrete walls ?

Sorry for my questions
and thanks again

Hello

I have verified what is implemented in the subroutine buse.f and I was wrong, I'm sorry.
The section is, in deed, taken as a rectagular shape which is computed using the width and the height HAUT (which is, in the pressurized case, the distance between the bed elevation and the lowest point of the bridge).

The upstream and downstream bed elevation are not necessary since, they can be deduced from tube's elevations (z1 and z2) and the height HAUT.
You can manage the diretion of the flow through the tube by setting the option Clp (0: both directions allowed, 1: flow from point 1 to point 2, 2: flow from point 2 to point 1 and 3: no flow at all)
You can have a look on subroutine buse.f (sources/telemac2d) to have more details.

I hope that this helps

with my best regards

Riadh ATA

Dear Forum:

I'm modelling a hypothetical urban area with a simple channel flowing through it. There's a bridge in the middle of the domain (see attachments).

I have modelled the bridge piers as holes ('islands') in the mesh, and have used a 'tubes' file to define the characteristics of the bridge openings between piers, the height of the bridge deck, etc.

Following the information in the user's manual v7p0, I didn't define any sources, but simply entered the global node numbers of the mesh nodes where each tube starts and ends. Is this correct?

My second question is: When the water level in the nodes that are below the bridge reaches the lower part of the bridge's deck (z1 + Hau or z2 + Hau), does the model automatically switch to pressure flow and turns off the shallow water equations for those nodes? Where do I find more details about this?

Should I rather delete those nodes?

Many thanks

Roberto

Hi,

There are two possibilities to model bridges.

1. Model the bed and the bridge opening directely in the mesh, as you did in your example. In that case you can model precisely the flow contraction in the bridge section in 2D BUT you cannot model pressurized flow (when the water surface becomes higher than the opening height) nor overflow on the deck. This method assumes that the bridge opening is not limited in the vertical direction.

2. Model only the discharge through the bridge with TUBES. For this method you need to model the bridge geometry across the river up to the deck elevation - like an embankment without openings (see test case \examples\telemac2d\bridge). The flow through the bridge is calculated by the subroutine buse.f for both free surface or pressurized flow. When the free surface becomes higher than the deck, then the overflow is simulated directly in 2D by solving the shallow water equations on the deck. The main disadvantages of this method is that you must define your opening section as a rectangule which is often too simplistic for real geometries and that approaching flow conditions are very simplified.

In short:
- if you are sure that the flow will not switch from free surface to pressurized flow through the bridge => method 1.
- otherwise, method 2. You can maybe use several tubes to subdivide one opening, but pay attention to the head loss coefficients.

Hope it helps!

Best regards
PL

Hello PL.

Thanks for your very useful response!

I have run my model and everything went fine. I don't want to simulate flow over the bridge deck, so I just made an island where the bridge is located and created two tubes, one for each bridge opening.

However, looking at the results (see attached pics), it seems that one of the tubes carries much more discharge than the other, even though they are exactly the same (project files attached).

Any hints are greatly appreciated.

Thanks again!!

Roberto

Hello,

I am on vacation so I only reply quickly... A few thoughts:

Your velocity map gives ONLY the velocity upstream and downstream of the tubes, not the discharge through them. If your bottom is deeper upstream of the southern tube then what you get does not sound illogical.

Do you reach a steady state?

What does the listing say? You should have, for each printout, the value through each tube, that's the best way to control your results.

Finally, don't forget that the "tube" function has some limitations:
- only rectangular dimensions
- discharge is computed based on water levels and not on energy levels as it should be in theory

The latter can maybe lead to some "oscillations" with the discharge alterning in the two tubes (possibily with high approaching velocities, just a guess, never tried such a configuration, I might be wrong) with for example:
- higher u/s water level at tube 1 => Q1 increases and Q2 decreases
- as Q1 increases, u/s velocity V1 also increases and water level decreases until WL 2 > WL 1, and same phenomenon at tube 2, and so on...

As a last word, I would actually use tubes to model a bridge only if I can't do it with the classical method (with openings in the mesh and the piles as island), ie. in the case when the flow is expected to reach the deck.

The best solution would be a coupled model 1D-2D Mascaret-TELEMAC-2D as bridges are easily modelled in 1D models (this works well with MIKE FLOOD with DHI software). But I don't know if a coupled version is in the pipe or not...

Best regards
PL