# Pressure Boundary Inlet and Outlet

 Register Blogs Members List Search Today's Posts Mark Forums Read

 March 28, 2017, 04:51 Pressure Boundary Inlet and Outlet #1 Senior Member   Join Date: Mar 2013 Location: Germany Posts: 357 Rep Power: 13 Hi All I am doing a pipe flow with diffuser at one end. I have a basic doubt about the Boundary condition to apply !! I know the inlet static pressure of 10 bar and corresponding mass flow rate of 15 L/min and there by the velocity as I know the Pipe inlet Diameter. So for Inlet I have ( Static Pressure, velocity, massflowrate) For outlet I dont have any information except that its going to atmosphere.So I take the Static Pressure at the outlet as 1 bar and reference Presseure as 1 bar So in my case I am applying Inlet : Static Pressure 10 bar Outlet Static pressure 1 bar Ref Pressure 1 bar By doing this I am forcing the simulation to this pressure values, and not specifying the velocity at all. So does this mean anything wrong or am I right , can I just give the pressure values alone ? When I give the mass flow rate at inlet and static pressure of 1 bar as outlet pressure I am getting an inlet pressure of 8bar. That means my pressure gradient is different. Or in otherways in actual case its 10 bar but I get 8 bar. So what can be the reason or what can we do. !!!

 March 28, 2017, 08:38 #2 Senior Member   Join Date: Jun 2009 Posts: 1,665 Rep Power: 29 Using static pressure on both inlet and outlet is a recipe for problems. The problem is mathematically ill-posed. The simplest example of ill-posed boundary conditions is the following: say inlet mass flow = 1 [kg], and outlet velocity specified. Such conditions are ill-posed since you must guarantee that for the given mesh, and material the integral of density * velocity * normal area exactly match the inlet mass flow. Say the material is also incompressible; therefore, the integral is subject to mesh resolution/quality to match the inlet mass flow value. Summary: the equation will have considerable trouble to converge, and they will NEVER converge to round off since there is a finite lack of conservation from the start. For your proposal, similar problem occurs because the momentum equation in a pipe flow is basically the force balance of the shear stress on the walls with the pressure gradient between inlet and outlet. Unless the specified pressure match exactly the discrete solution for that mesh, there will be a finite lack of conservation of linear momentum. You must use either total pressure and static pressure outlet, or a mass flow condition on either side. Hope the above helps, kaifu, Shanaylla and rtyme06 like this.

 March 28, 2017, 09:06 #3 Senior Member   Join Date: Jun 2009 Posts: 1,665 Rep Power: 29 duplicate, pressed save twice

 March 28, 2017, 09:11 #4 Senior Member   Join Date: Mar 2013 Location: Germany Posts: 357 Rep Power: 13 Well thats what atleast I was thinking but unfortunately or fortunately my simulations were converged (RANS) So my doubt is Ok I know the Total pressure at the Inlet (10.08 bar) Outlet (Static Pressure ) Atmosphere = 0 bar as my reference pressure =1 bar But my doubt is should I reduce this 1 bar in my Total pressure as well ? As I am giving reference pressure of 1 bar ? Inlet (total Pressure)= 10.08bar outlet =1 bar Ref =0 bar Since gicing 0 bar as reference is not good we give 1 bar so my inlet becomes Inlet = 9.08 bar Outlet = 0 bar and Ref Pressure = 1 bar ?? OR should I keep the Inlet (total)Pressure as 10.08 ?

 November 7, 2017, 05:54 #5 Member   ehsan Join Date: Sep 2014 Posts: 38 Rep Power: 10 Dear Opaque, What about using the pressure conditions at both ends (inlet and outlet) while using the coupled algorithm (instead of SIMPLE). Is it still overdetermined? For instance, if we have an unsteady pipe flow with deposition what would be a proper BC for inlet? ( due to deposition we would face an increasing flow blockage inside the pipe and increasing pressure drop leads to the mass flow reduction). Best regards, Ehsan

 March 28, 2018, 10:46 #6 New Member   Aadit Shroff Join Date: Mar 2018 Posts: 3 Rep Power: 7 Hello! I am facing a very similar issue. I am simulating a transient flow (water) through a choke valve (in SimScale) using the PIMPLE solver. I have only the following conditions known to me: 1) Inlet Pressure - 8.27 MPa (gauge) 2) Inlet Mass Flow Rate - 5.52 kg/s 3) Inlet Temperature - 65.5 C My objective is to find the pressure drop across the valve. For this I have calculated the flow velocity at the inlet through the mass flow rate (m*=roh.A.V) which I supply as the inlet velocity BC. Outlet pressure BC is set to 0 Pa gauge (hence, exhausting to the atmosphere). Is my approach correct? In this case, when I get the pressure results, does it mean that the highest pressure value is the total drop in pressure? Does specifying the inlet velocity automatically take the pressure into account? When I set the inlet BC as the inlet pressure, I get insanely high valves of pressure and velocity in the valve. Is there any way I can use the pressure inlet BC and still run a simulation? I mean, could I use the inlet pressure and outlet mass flow as my BC combination? (inlet and outlet mass flow are the same as the valve has no leakage.) Looking for general advise regarding this as I am very new to CFD. Thank you! Regards, Aadit