
[Sponsors] 
October 28, 2014, 05:00 
velocity boundary condition at inlet and outlet

#1 
Senior Member

Join Date: Oct 2010
Posts: 303
Rep Power: 9 
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.
__________________
Best regards, Santhosh. 

October 28, 2014, 06:15 

#2 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 11,575
Rep Power: 90 
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. 

October 28, 2014, 06:27 

#3 
Senior Member

Join Date: Oct 2010
Posts: 303
Rep Power: 9 
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.
__________________
Best regards, Santhosh. 

October 28, 2014, 06:45 

#4 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 11,575
Rep Power: 90 
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.


October 31, 2014, 02:05 

#5 
Senior Member

Join Date: Oct 2010
Posts: 303
Rep Power: 9 
Hi Glenn,
Many thanks for the clarification, as always your generosity is of appreciable help.
__________________
Best regards, Santhosh. 

February 2, 2015, 12:11 

#6  
Senior Member
Join Date: Aug 2014
Posts: 149
Rep Power: 3 
Quote:
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/ valvetype 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. 

February 2, 2015, 17:35 

#7 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 11,575
Rep Power: 90 
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. 

February 3, 2015, 02:52 

#8  
Senior Member
Join Date: Aug 2014
Posts: 149
Rep Power: 3 
Quote:
A quick ask to resolve this further, I have also observed that whether using the density CEL expression [1000 [kg m^3]/(1(p101325[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. 

February 3, 2015, 17:48 

#9 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 11,575
Rep Power: 90 
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.


February 11, 2015, 09:24 

#10  
Senior Member
Join Date: Aug 2014
Posts: 149
Rep Power: 3 
Quote:
Hopefully one of the last selfdumbchecks 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(p101325[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. Last edited by fresty; February 11, 2015 at 09:57. Reason: conceptual mistake 

February 11, 2015, 18:21 

#11  
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 11,575
Rep Power: 90 
Quote:
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)^21/2*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. 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Wind turbine simulation  Saturn  CFX  45  Yesterday 05:42 
ATTENTION! Reliability problems in CFX 5.7  Joseph  CFX  14  April 20, 2010 15:45 
RPM in Wind Turbine  Pankaj  CFX  9  November 23, 2009 05:05 
Convective Heat Transfer  Heat Exchanger  Mark  CFX  6  November 15, 2004 16:55 
what the result is negatif pressure at inlet  chong chee nan  FLUENT  0  December 29, 2001 06:13 