[pa8001]

I am trying to simulate a hydraulic jump in open channel flow, how can I force the flow to stay in sub critical condition at the downstream during the simulation.
when I use pressure inlet and pressure outlet BC, after running the model the velocity and depth of the flow in inlet and outlet do not stay fixed and the model changes the BC.
I also have tried velocity inlet and the pressure outlet, but after running the model will not keep the velocity and depth at the outlet fixed.

could someone plz help me how to set the BC for simulating hydraulic jump in open channel flow?

thanks

[Ema40]

Hi.

If the outlet BC does not remain fixed, probably because it is not right. But you are simulating steady or unsteady simulation?

[pa8001]

Originally Posted by Ema40

Hi.

If the outlet BC does not remain fixed, probably because it is not right. But you are simulating steady or unsteady simulation?

Thank you ema!
It is unsteady. I use pressure outlet Bc for downstream as an openchannel. But I dont know how to impose a fix depth during the simulation

[Ema40]

hi..you have fixed also the upstream depth?

[kbaker]

Hi pa8001 if you want fix level why you not try patch the secondary phase from inlet until outlet? I do not know exactly what you mean here by depth? is it same as free surface level?

[pa8001]

hi kbaker
yes exactly I mean the free surface level. how can I patch the secondary fase when my water surface level at the inlet is 15cm and at the outlet is 80cm?

[kbaker]

I think here you need to find the equation of variation of vof with distance and write it in UDF? if the level is a linear its a simple linear equation else if it a curve you need equation from second degree? But why you just try use 15 cm at inlet pressure boundary as level and 80 cm at pressure outlet ? what the problem with using these setting with open channel flow boundary with you?

[pa8001]

the problem is that, when i set the 15cm in the inet and 80cm in the outet, if i set 15 cm for the initial water surface level all over the channel, at the first timestep after 0 model will change the depth of donstream boundary from 80 to 15. if i initialize the water surface level a ll over the channel to 80 cm, the model will change the inlet water surface level from 15 to 80 cm at the firt time step after 0.
just to let you know, i want to produce a simple hydraulic jump. i need my inlet flow as super critical and the outlet flow as subcritical.

thank you for your help

[sebastianbn]

Originally Posted by pa8001

the problem is that, when i set the 15cm in the inet and 80cm in the outet, if i set 15 cm for the initial water surface level all over the channel, at the first timestep after 0 model will change the depth of donstream boundary from 80 to 15. if i initialize the water surface level a ll over the channel to 80 cm, the model will change the inlet water surface level from 15 to 80 cm at the firt time step after 0.
just to let you know, i want to produce a simple hydraulic jump. i need my inlet flow as super critical and the outlet flow as subcritical.

thank you for your help

Hey! Did you find any solution?
I'm trying to represent this exact problem and it happens the same, my outlet boundary condition (subcritical flow) ends having the exact same height as my inlet (supercritical flow).

Thanks in advance!

[masoud.ravan]

I have this problem with simulating open channel flow? does anyone know how to use "open channel flow" submodel???
Thanks in advance

[l.whelan11]

Hey, I was having this issue as well recently, I think I may have a solution. I replied to my own thread here:

Acceptable residuals of continuity in open channel flow?

[sebastianbn]

Originally Posted by l.whelan11

Hey, I was having this issue as well recently, I think I may have a solution. I replied to my own thread here:

Acceptable residuals of continuity in open channel flow?

Hey!

I also found a solution without using two sets of boundary conditions. What I did was to set my inlet face to the same height as my upstream pressure inlet, as if there was a gate controlling the flow entrance, and setting the rest of this face ("gate") as a wall.
With this, both my inlet and outlet heights remain as the boundary conditions I gave at the beginning.

Now the problem I'm having is that I don't undertand why this is occuring... I shouldn't be redundant with the inlet condition (setting the inlet height just as the upstream free surface level) or at least that's what I think...
Also if I set the "gate" at a higher level and keep my free surface level equal, it still works. Which is very rare since the "gate" is not in contact with the flow.
Does anyone have any clue of why does this happen?

[l.whelan11]

Originally Posted by sebastianbn

What I did was to set my inlet face to the same height as my upstream pressure inlet, as if there was a gate controlling the flow entrance, and setting the rest of this face ("gate") as a wall.

Hi Sebastian,

Sounds interesting! Could you maybe post a phase plot or similar to give an idea of the setup? I'm just struggling a bit to visualise it! Although I am almost finished with this project so I won't be changing mine anyway :P

[sebastianbn]

Originally Posted by l.whelan11

Hi Sebastian,

Sounds interesting! Could you maybe post a phase plot or similar to give an idea of the setup? I'm just struggling a bit to visualise it! Although I am almost finished with this project so I won't be changing mine anyway :P

Hey!

I'm studying near-critical flow in a partially filled pipe, what I'm doing is reproducing an undular hydraulic jump a keeping the froude numbers very near to 1.

Here is a screenshot of the inlet condition I'm using, and is shown the gate, the free surface lavel and the gap that exists between them (wish I say, with this gap the simulation shouldn't work but it does...)
Inlet.jpg
And here is the phase profile, which is the one expected and was obtained from this inlet condition:
Profile.jpg

Doing a little bit of research, I found out this in the FLUENT User's Guide - 23.10.2. Modelling Open Channel Flows:

"The initialization procedure is very critical in the open channel analysis. If you are interested in the final steady state solution, then perform the following initialization procedure:

1. Initialize the domain by setting the volume fraction of the secondary phase to 0, and providing the inlet velocity.
2. Patch the domain using a volume fraction value of the secondary phase to 1, up to the Free Surface Level specified at the inlet.
3. Patch the inlet velocity again in the full domain.

If the Free Surface Level values are different at the inlet and outlet, then patching some regions with inlet Free Surface Level values and some regions with outlet Free Surface Level values could be useful for some problems"


Although this is not absolutely clear to me right now... I think this may be the "correct" answer to this thread.
If anyone could give out an example of this procedure or anything it would be very helpful!

Cheers