Hi all,
I freed my brain and got it. The p_rgh field is not the static pressure minus the hydrostatic part as the reference height is always different. Thatīs why we name it "working" pressure. However, some small hints:
|
Hi Tobi!
How do you mean that the reference height is always different? It is zero by default. Also the prghPressure BC uses the hRef value from the db() so it will be the same again. I think hRef is always the same. Sorry if this is a stupid question, but you made me a bit confused now :D And what was the solution for your problem? (just to clarify :) ) |
Yes hRef is always set to zero by default. I am sorry for not describing it well. Lets talk about my case above. For me the reference is always the top level of the liquid. Means in my case, the top of the big storage tank. My reference value for analystic calculation should be set to 3m here. Therefore, the hydrostatic part (rho g h) will increase with respect to the top patch of the big storage tank (:
You are right, the reference height is always set to zero. However, if you move the geometry 2 m up or down, the p_rgh value will change accordingly (which made me always a bit messed up). The solution is as follows (not 100 % clear for me now): - Setting up prghTotalPressure for the inlet (1e5 Pa) - Setting up prghPressure for the outlet (1e5 Pa) - Setting hRef to 3 m It follows: p_rgh at the inlet is equal to the static pressure corrected by the fluxes (in this boundary condition no rho g h is used as the prghTotalPressure is equivalent to totalPressure) p_rgh at the outlet is equal to the static pressure - rho g dh (~2 m) Thus, the driving force is the difference. Nevertheless, I thought that the potential energy difference (rho g h) from top patch of the inlet to the outlet will relate to the velocity we achieve. I will try to make a clear statment: Position 0 (inlet; top patch of large tank Position 1 (outlet) Bernoulli Energy at Position (1) is equal to (2): infinit large tank Therefore, it follows: However, I do not reach this velocity at all. Right now I have 0.6 m/s (not converged yet). |
1 Attachment(s)
I just made a toy case. Please don't check the turbulent BCs, random numbers... And mostly not a really correct case. BUT!
Fluid: water deltaH: 3m calculated velocity: 7.672 m/s resulted max velocity at outlet: 7.6861 m/s case:
here, (prescribed total pressure) (prescribed static pressure) thus , the same as you did. toy case attached. (WARNING! Really poor case, but correct results. At least I accept it. :D) |
Did not check the case right now but I agree that the inlet boundary condition should be totalPressure (or prghTotalPressure) in order to reduce the pressure gradient based on the fluxes.
You case should accelerate the fluid until infinty and crash if you set a staticPressure to the inlet too. Thank you very much for investigating into my "simple" topic. I will check you case now. |
Hi Tobias,
I realise that this tread is old, but I hope you are able to answer my question. You state that ph_rgh is not available, which is also my experiance. Do you have any idea in which cases the boundary condition should be used? Btw, looking at your geometry it makes sense that you do not reach the velocity of 6.26 m/s. In the flow you have two sudden contractions, two sharp edges and two sudden expansions. Especially the first two come with a pressure drop. Regards, Lourens |
Hi,
I did not further investigate into that topic but probably we could resolve the issue I had by using the prghTotalHydrostaticPressure boundary condition or a normal one but initialize the case by using the hydrostaticPressure FO. Tobi |
Hi Tobias,
If I do understand well: the prghTotalHydrostaticPressure is a constant prgh boundary condition corrected for Bernoulli. What I do not understand is the meaning of the ph_rgh term in the equation. It looks like a way to describe the pressure at the boundary to be used for e.g. water flowing out of a container. This is confusing me, since I expected a p_rgh boundary to be there for buoyant flows (e.g. natural convection is a room). What is also confusing me, is that the value of ph_rgh inthe equation is seems to be a function of the local density. If the differences in density are small over height, this a good approximation. If not an integral over height should be used. What do you mean by "initialize the case by using the hydrostaticPressure FO"? What exactly was your issue? Lourens. |
Hi Simrego,
I did run your test case but it blew up in OF 7. I tried to refine your mesh 10 times but at around 9,600 iterations, it blew up again. The maximum velocity in the outlet at that time is still around 6.4 m/s. I don't understand why your simulation ran pretty well. -Mike |
All times are GMT -4. The time now is 07:18. |