Pressure and Velocity boundary conditions
Hello all!
I've presented my last results last week for some teachers and one of them has made me a question which I cannot answer. I've been simulating a flow in a straight pipe (100 D) and in the same straight pipe with one and two bends upstream of it. I've been using ANSYS CFX v.13. Boundary conditions have been inlet uniform velocity and outlet average static pressure to all cases. I've been questioned about what would be the boundary conditions for pressure at the inlet and velocity at the outlet. This teacher has experience in CFD but is not used to CFX modeling. He defends the idea that any mathematical condition for both velocity and pressure is necessary at all domain boundaries. He also said that, probably, CFX has already the condition of full developed flow at the outlet. Once the two bend case simulated has not presented fully developed flow at the outlet he questioned if thah result was correct. Could anyone of you guys tell me if he is right or wrong and how CFX treats boundary conditions? Do I have to extend the outlet condition downstream in order to find fully developed condition? If only inlet velocity and outlet pressure conditions are necessary, how it works on CFX? How the solver finds and treats pressure and velocity at inlet and outlet, respectively. Best regards, Ramon Silva Martins P.S.: Sorry if it's already been discussed. I couldn't find. 
The flow boundaries which are implemented in CFX are fundamentally of two types  velocity and pressure. Which ever is defined, the solver works out the other. CFX does not give you the option to specify both at a single boundary. But read the documentation  when you specify pressure it applies a zero normal gradient constraint on the momentum so you are putting constraints on both pressure and velocity.
If you want the fully developed condition then it sounds like you need to go further downstream. But you can also do this using a periodic pair with a defined flow rate, so then you can get the fully developed flow with a short domain. 
Hello Glenn. Thank you very much for your answer.
I could not find any information about the constraint on the momentum equation when average pressure is specified at the outlet in the documentation. Could you point me that? Still, since we started the discussion, I would like to reformulate my question. Actually, I would like to know if it is OK if the domain outlet is located where fully developed flow is not achieved yet? How does CFX treat or calculate it then? What are the mathematical conditions to the momentum equation at this boundary? I'm still searching and studying to try to understand that... I appreciate your attention again. Regards, Ramon Silva Martins 
The outlet condition (in pressure mode) simply applies the specified pressure and zero normal gradients on most other variables. This is accurate in fully developed flow but does cause an issue where the flow is not fully developed (ie the normal gradients are not zero). But having said that for most engineering calculations this is a minor consideration and the accuracy loss is insignificant.
This is all described in the documentation. 
Did anybody find that part about the constraints on the momentum equations during the last four years? :) I was also looking for it and the only thing i found was that:
This option also requires that the Flow Direction is specified, and is used if the flow is into the domain. For details, see Flow Direction. If I set flow direction "normal to boundary", for continuity reasons, the gradient normal to the boundary must be zero. However, the documentation states that this used if the flow is into the domain. To me that means it is not used if the flow is out of the domain. I would generally agree Ramon's teacher that I do need a boundary condition for the velocity if i solve a differential velocity equation. But the CFX documentation is not really clear about that... at least in my understanding. 
What do you mean constraints on the momentum equation? The pressure averaging procedure is described in the documentation. So what is not clear from that?
A correction to my previous post  the documentation says for other variables at an outlet boundary it applies a constant gradient (generally nonzero). My understanding was that it just convected the variable out of the domain, however this suggests it applies a constant gradient. I do not understand what the documentation means by this constant nonzero gradient. 
Quote:

Are you referring to opening boundaries?
The documentation states that the flow direction is required because the inflow direction uses the total pressure. Thus the flow velocity is required and a direction needs to be defined for it. If the flow is out of the domain then the boundary pressure is set to the static pressure defined, and no gradient need be defined. If I have misunderstood your question please clearly state whether you are talking about inlets,outlets or openings and which form of it. 
I skipped the word "outlet" that you used. My bad! I'm more interested in the mathematical background of the opening bc, specifically in the "opening pressure and direction" or "static pressure and direction" form. But in the end it might be a general question.
I understand that the velocity gradient (or the flow direction) is not defined at an opening when there is only outflow. But that brings the statement of rsmartins' teacher up: "any mathematical condition for both velocity and pressure is necessary at all domain boundaries." At first glance this statement makes sense to me since there is a pressure derivative and a velocity derivative in the system of differential equations that we are solving, so I thought we need a boundary condition for both. Can you explain where my error in reasoning is? edit: Above you mentioned, that the flow boundaries which are implemented in CFX are fundamentally of two types  velocity and pressure. Which ever is defined, the solver works out the other. Does that also apply for noslip wallboudaries? I assumed that there was a dp/dn = 0 boundary condition at walls, which is unphysical in some cases. But if specifying the velocity is enough and the pressure is part of the solution, than I get why the documentation does not state anything about the pressure on wall boundaries. 
The CFX documentation does not go into details like what pressure boundary it uses on walls. But I am pretty sure it is dp/dn=0. And you are correct, for a small number of flows this is not correct (generally very low Re flows in my experience, but could be others)
Likewise at an inlet or outlet where you have specified the velocity the CFX documentation does not state what it does for the pressure. I presume that it applies dp/dn=0 again, but I cannot be sure of this. 
All times are GMT 4. The time now is 05:54. 