Setting a inlet pressure boundary condition

I want to set up pressure boundary conditions both for inlet and outlets of my geometry model. But, I did not find how to do that for inlet. Only inlet /  velocity condition is possible in FEATool ?

Please suggest.

rvrmohan wrote

I want to set up pressure boundary conditions both for inlet and outlets of my geometry model. But, I did not find how to do that for inlet. Only inlet /  velocity condition is possible in FEATool ?

The inlet/outlet designations are just labels for the normal or typical use of these boundary conditions. When you prescribe either velocities or pressure it depends on the actual values you prescribe wether the resulting boundary will result in inwards or outwards fluid flow (and the rest of the model). If you for example prescribe negative velocities on an inlet/velocity boundary (with respect to the outward normal of the boundary) it will effectively function as an outlet, and if you have one boundary with higher pressure than the others it should also act as an inlet.

My geometry has two boundaries, which I am setting as pressure boundaries. I am setting boundary 84 as outlet / pressure boundary (10000 mm water column) and 89 as outlet / pressure again (0 mm, atmospheric). All other boundaries are solid no-slip boundaries. Pl see: 1_inlet_pressure_boundary_condition.PNG.

1. When I choose any of the Turbulence models - k-e, k-e (RNG), k-e (realizable), k-omega - using OpenFOAM, from equation mode and try to 'edit' the inlet conditions, it shows me an error: 2_inlet_conditions_not_detected_error.PNG. Further, when I go ahead to 'solver mode' and click solve on OpenFOAM, it gives me this error: 3_error_for_OpenFOAM_k-e_turbulence_model.PNG.

2. When I choose any of the Turbulence models - Laminar, Spalart-Allmanas, k-omega(SST) - using SU2, and try to 'edit' the inlet conditions, it shows a similar error as above - 'inlet conditions not detected'. Further, when I go ahead to 'solver mode' and click solve on SU2, it gives me this error: 5_SU2_solver_error_message.PNG.

Therefore, though the inlet / outlet designations are just labels, but for external solvers, it does pass on inlet conditions resulting in errors and solver failures.

Am I right or is there anything that I am missing ?? Please help out.

rvrmohan wrote

1. When I choose any of the Turbulence models - k-e, k-e (RNG), k-e (realizable), k-omega - using OpenFOAM, from equation mode and try to 'edit' the inlet conditions, it shows me an error: 2_inlet_conditions_not_detected_error.PNG. Further, when I go ahead to 'solver mode' and click solve on OpenFOAM, it gives me this error: 3_error_for_OpenFOAM_k-e_turbulence_model.PNG.

To estimate turbulence quantities over inlet boundaries the mean velocity "u_mean" over the boundary is used, specifically

    k = 3/2*( u_mean * turbulence_intensity )^2
    epsilon = C_MIU^3/4*k^3/2 / turbulent_length_scale  
    omega = C_MIU^-1/4*k^1/2 / turbulent_length_scale  

which is not present for pressure boundaries.

rvrmohan wrote

2. When I choose any of the Turbulence models - Laminar, Spalart-Allmanas, k-omega(SST) - using SU2, and try to 'edit' the inlet conditions, it shows a similar error as above - 'inlet conditions not detected'. Further, when I go ahead to 'solver mode' and click solve on SU2, it gives me this error: 5_SU2_solver_error_message.PNG.

Therefore, though the inlet / outlet designations are just labels, but for external solvers, it does pass on inlet conditions resulting in errors and solver failures.

Unlike FEATool (and FEniCS), the SU2 and OpenFOAM external CFD solvers are not set up to handle problems without defined inlet boundaries which are not detected with just fixed pressure boundaries. You can use the "Export" functionality to export the configuration/case files and manually edit them to correct for this.

For example for the corresponding SU2 .cfg configuration file you would most likely change/prescribe "INC_INLET_TYPE= VELOCITY_INLET" to "INC_INLET_TYPE= PRESSURE_INLET".

Thanks for this insightful advise. I understand now how different solvers treat pressure boundaries.

In my case, I do not need solutions at a particular pressure value at the inlet. I want to obtain discharge / flux at the outlet for different pressure values at the inlet and establish an empirical relation between them using regression analysis.

I have two specific questions in this regard:

1. I assign velocity at the inlet boundary condition and solve N-S equation with turbulence models of SU2 and OpenFOAM. Then, quantify avg pressures at inlet and avg discharges at the outlet for each velocity value at inlet using boundary integration option in post-processing menu. This way, I could use all the turbulence models. Whether this approach is acceptable and scientific ?

2. For calculating the discharge at the outlet using boundary integration,whether I have to consider mean velocity (sqrt(u^2+v^2)) or the 'u' in x-direction alone ?

Your advise will help a lot. Thanks a lot for your patient and prompt replies.

rvrmohan wrote

1. I assign velocity at the inlet boundary condition and solve N-S equation with turbulence models of SU2 and OpenFOAM. Then, quantify avg pressures at inlet and avg discharges at the outlet for each velocity value at inlet using boundary integration option in post-processing menu. This way, I could use all the turbulence models. Whether this approach is acceptable and scientific ?

If I understand your approach correcly, you intend to "iteratively" adjust the inlet flow until you achieve your desired pressure drop? This would certainly be a valid approach although not as efficient (as you would solve the model several times). An update will be released to allow for pressure inlets for OpenFOAM and/or SU2. As you maybe have noticed it often does not work too well with just pressure conditions in FEA simulations such as FEATool, due to the fact that one needs to prescribe a "periodic pressure drop" (not just assign pressure values), this can be done on the command line using a "solver hook" as for example in the ex_navierstokes14 script model.

rvrmohan wrote

2. For calculating the discharge at the outlet using boundary integration,whether I have to consider mean velocity (sqrt(u^2+v^2)) or the 'u' in x-direction alone ?

Yes, I think it would typically be more appropriate to use all velocity components.