[saisanthoshm88]

I'm dealing with a transient simulation with a single inlet and multiple outlets. Water (incompressible liquid) is the working fluid.

I know that using a velocity boundary condition at both inlet and outlet will result in an ill posed system.

But I'm not sure if that is the case with transient simulations also, could some one please clarify on this, because right now I have mass flow at the inlet and velocities at the outlets as the available information.

[ghorrocks]

Have a think about it - if a small numerical error occurs in a boundary, what can the simulation do to offset it? In a compressible simulation it can change the density of the gas slightly. In a incompressible simulation it cannot do anything so it will crash. Ergo, your simulation is invalid.

But the fix is simple. You know the flow rate in and the velocities at multiple outlets. The flow rate in is redundant as you already know that from the outlets, so make this a pressure inlet set to zero gauge pressure. The mass flow rate at the inlet will be correct due to mass continuity, pressures will be relative to the inlet and your simulation is well posed. It's all good.

[saisanthoshm88]

Hi Glenn,

Thank you very much for the clarification, I have run the transient simulation by using mass flow at the inlet and respective velocities at different outlets.

The transient simulation ran fine without crashing but of course I do not have the possibility to cross check if the results are all physical.

But of course I comprehend the point that in case of using such inlet mass flow and outlet velocity conditions, the solver lacks information on the pressure and that this can lead to an ill posed set up.

So I'm actually wondering why my simulations didn't show up a problem.

[ghorrocks]

Whether the solver crashes or fails to converge depends on the details of the numerical method. I bet if you look at your imbalances they will not have converged - and they never can. If you fix the inlet and outlet flow rates then any small difference in the flow rate can never be corrected.

[saisanthoshm88]

Hi Glenn,

Many thanks for the clarification, as always your generosity is of appreciable help.

[fresty]

Originally Posted by ghorrocks

Whether the solver crashes or fails to converge depends on the details of the numerical method. I bet if you look at your imbalances they will not have converged - and they never can. If you fix the inlet and outlet flow rates then any small difference in the flow rate can never be corrected.

Hi Glenn,

I was just looking for something similar but basic help related to well posed boundary conditions in my simulation model (dealing with mass flow inlet & outlet) and probably reached a point where I fear posting a stupid but very desperate question for your help.

My constraint is mass flow rate at inlet and equal mass flow rate at the outlet, this is to observe consequent pressure drop in the transient compressible system/ valve-type model. During a cross check (removing the compressibility CEL density expression used for pressure pulse model), I have observed that imbalanced specification of mass flow rate at inlet/ outlet boundary does not generate error; is it not against the Mass continuum in theory? As now the the flow in incompressible, doesn't that call for equal mass flow inlet & outlet else would crash/ diverge..? Your quick comment could clear this doubt.

Cheers.

[ghorrocks]

In a compressible transient simulation the flow in does not need to equal the flow out as material can accumulate in the domain. In a incompressible transient simulation the flow in and out will not always balance if there is mesh motion. But assuming that does not apply then it suggests that your incompressible simulation with a difference between inlet and outlet flow has a significant imbalance.

By default CFX just uses the residual to define convergence. In some cases you need to set the imbalances as an additional convergence criteria. It sounds like you need this in your case as it sounds like your simulation is not fully converged.

[fresty]

Originally Posted by ghorrocks

In a compressible transient simulation the flow in does not need to equal the flow out as material can accumulate in the domain. In a incompressible transient simulation the flow in and out will not always balance if there is mesh motion. But assuming that does not apply then it suggests that your incompressible simulation with a difference between inlet and outlet flow has a significant imbalance.

By default CFX just uses the residual to define convergence. In some cases you need to set the imbalances as an additional convergence criteria. It sounds like you need this in your case as it sounds like your simulation is not fully converged.

Thanks a lot Glenn. That clears it all and yes like you said & i realized that my simulation is not fully converged (talking in terms of residuals) in case of incompressible flow (with forced/ specified mass flow imbalance at boundaries).
A quick ask to resolve this further, I have also observed that whether using the density CEL expression [1000 [kg m^-3]/(1-(p-101325[N m^-2])/2150000000[N m^-2])] or not for even a simple flow through a Tube/ Cylindrical domain ends up generating different (imprecise) results. Shouldn't it be (sorry if i am wrong on this) that compressibility CEL is an ideal condition (density based formulation for ideal gas/ flow) and all incompressible fluid simulations should generate similar results (with or without this CEL).
Apologies if the question is slightly vague.

Thanks.

[ghorrocks]

Variable density means another factor you need to converge and get accurate. A fully converged and accurate simulation with variable density will be more accurate than an incompressible simulation as it is closer to reality. But it does make convergence harder. So I suspect your inaccuracy is more to do with poor convergence.

[fresty]

Originally Posted by ghorrocks

Variable density means another factor you need to converge and get accurate. A fully converged and accurate simulation with variable density will be more accurate than an incompressible simulation as it is closer to reality. But it does make convergence harder. So I suspect your inaccuracy is more to do with poor convergence.

Hi there again Glenn,

Hopefully one of the last self-dumb-checks from me (for this model!).


The CEL I used for the variable density/ slightly compressible nature of water (to observe pressure waves) is:

1000 [kg m^-3]/(1-(p-101325[N m^-2])/2150000000[N m^-2])

The question would be, that by increasing the value of initial density the pressure drop (difference) of the system should increase, is this correct? However, by using higher density of 1200 [kg m^3], the pressure drop does decrease in my simulation. I understand that this changed input in value is not independent & all intrinsic properties of the fluid should also change (Bulk Modulus of Fluid). However, would still think that physically the pressure difference should be more with the increase in density of fluid? Your comments on this would help a lot.

[ghorrocks]

that by increasing the value of initial density the pressure drop (difference) of the system should increase, is this correct?

You will have to explain this better. What initial density? What pressure drop? A drawing would help.

Are you asking whether in general a steady flow through a device with a pressure drop should result in more pressure drop if the density of the fluid is increased?

Have a look at Bernoulli: p(in)-p(out) = 1/2*rho*V(out)^2-1/2*rho*V(in)^2. If V stays the same and rho (density) increases then p(in)-p(out) will increase. So the first order effects show the pressure drop will be proportional to the fluid density. Lower order effects (turbulence, high Re effects etc) will deviate from this a bit but for low speed flow it will be pretty close.

[CFDnerd]

Originally Posted by ghorrocks

Have a think about it - if a small numerical error occurs in a boundary, what can the simulation do to offset it? In a compressible simulation it can change the density of the gas slightly. In a incompressible simulation it cannot do anything so it will crash. Ergo, your simulation is invalid.

But the fix is simple. You know the flow rate in and the velocities at multiple outlets. The flow rate in is redundant as you already know that from the outlets, so make this a pressure inlet set to zero gauge pressure. The mass flow rate at the inlet will be correct due to mass continuity, pressures will be relative to the inlet and your simulation is well posed. It's all good.

I am running a similar analysis with 1 inlet and 3 outlets. i am using inlet velocity, outlet mass flow and two outlets as opening. These BCs are certainly well posed since openings will accommodate any flow fluctuations. Still my convergence is slow. The reason I am using mass flow at outlet is because I know how much mass is going out.

To improve convergence, I am planning to use pressure at the outlet instead of mass flow (while keeping two openings) since this is the most robust BC combination per CFX documentation. Will that affect the mass flow at that outlet significantly compared to the mass flow rate that I am using? Any recommendations on this will be appreciated.

[ghorrocks]

Yes, that simulation sounds well-posed.

Whether changing the outlet from pressure to mass flow has an effect depends on the system. If the mass flow rate generated from the pressure boundary matches the mass flow rate you applied then it should not have much effect.