CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

velocity boundary condition at inlet and outlet

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   October 28, 2014, 04:00
Default velocity boundary condition at inlet and outlet
  #1
Senior Member
 
---------
Join Date: Oct 2010
Posts: 303
Rep Power: 17
saisanthoshm88 is on a distinguished road
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.
saisanthoshm88 is offline   Reply With Quote

Old   October 28, 2014, 05:15
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,688
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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.
ghorrocks is offline   Reply With Quote

Old   October 28, 2014, 05:27
Default
  #3
Senior Member
 
---------
Join Date: Oct 2010
Posts: 303
Rep Power: 17
saisanthoshm88 is on a distinguished road
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.
saisanthoshm88 is offline   Reply With Quote

Old   October 28, 2014, 05:45
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,688
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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.
ghorrocks is offline   Reply With Quote

Old   October 31, 2014, 01:05
Default
  #5
Senior Member
 
---------
Join Date: Oct 2010
Posts: 303
Rep Power: 17
saisanthoshm88 is on a distinguished road
Hi Glenn,

Many thanks for the clarification, as always your generosity is of appreciable help.
__________________
Best regards,
Santhosh.
saisanthoshm88 is offline   Reply With Quote

Old   February 2, 2015, 11:11
Default
  #6
Senior Member
 
Join Date: Aug 2014
Location: UK
Posts: 213
Rep Power: 12
fresty is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
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.
fresty is offline   Reply With Quote

Old   February 2, 2015, 16:35
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,688
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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.
ghorrocks is offline   Reply With Quote

Old   February 3, 2015, 01:52
Default
  #8
Senior Member
 
Join Date: Aug 2014
Location: UK
Posts: 213
Rep Power: 12
fresty is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
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.
fresty is offline   Reply With Quote

Old   February 3, 2015, 16:48
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,688
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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.
ghorrocks is offline   Reply With Quote

Old   February 11, 2015, 08:24
Default
  #10
Senior Member
 
Join Date: Aug 2014
Location: UK
Posts: 213
Rep Power: 12
fresty is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
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.

Last edited by fresty; February 11, 2015 at 08:57. Reason: conceptual mistake
fresty is offline   Reply With Quote

Old   February 11, 2015, 17:21
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,688
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Quote:
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.
ghorrocks is offline   Reply With Quote

Old   August 2, 2018, 14:16
Default
  #12
New Member
 
CFDnerd
Join Date: Aug 2018
Posts: 5
Rep Power: 7
CFDnerd is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
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.
CFDnerd is offline   Reply With Quote

Old   August 2, 2018, 21:21
Default
  #13
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,688
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Wind turbine simulation Saturn CFX 58 July 3, 2020 01:13
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 04:05
Convective Heat Transfer - Heat Exchanger Mark CFX 6 November 15, 2004 15:55
what the result is negatif pressure at inlet chong chee nan FLUENT 0 December 29, 2001 05:13


All times are GMT -4. The time now is 08:58.