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

Pressure Boundary Inlet and Outlet

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

Like Tree3Likes
  • 3 Post By Opaque

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 28, 2017, 04:51
Default Pressure Boundary Inlet and Outlet
  #1
Senior Member
 
Join Date: Mar 2013
Location: Germany
Posts: 357
Rep Power: 14
AS_Aero is on a distinguished road
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. !!!
AS_Aero is offline   Reply With Quote

Old   March 28, 2017, 08:38
Default
  #2
Senior Member
 
Join Date: Jun 2009
Posts: 1,804
Rep Power: 32
Opaque will become famous soon enough
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.
Opaque is offline   Reply With Quote

Old   March 28, 2017, 09:06
Default
  #3
Senior Member
 
Join Date: Jun 2009
Posts: 1,804
Rep Power: 32
Opaque will become famous soon enough
duplicate, pressed save twice
Opaque is offline   Reply With Quote

Old   March 28, 2017, 09:11
Default
  #4
Senior Member
 
Join Date: Mar 2013
Location: Germany
Posts: 357
Rep Power: 14
AS_Aero is on a distinguished road
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 ?
AS_Aero is offline   Reply With Quote

Old   November 7, 2017, 05:54
Default
  #5
Member
 
ehsan
Join Date: Sep 2014
Posts: 38
Rep Power: 11
e_cfd is on a distinguished road
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
e_cfd is offline   Reply With Quote

Old   March 28, 2018, 10:46
Default
  #6
New Member
 
Aadit Shroff
Join Date: Mar 2018
Posts: 3
Rep Power: 8
aadit.shroff is on a distinguished road
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
aadit.shroff 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
Wrong flow in ratating domain problem Sanyo CFX 17 August 15, 2015 06:20
An error has occurred in cfx5solve: volo87 CFX 5 June 14, 2013 17:44
RPM in Wind Turbine Pankaj CFX 9 November 23, 2009 04:05
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 12:48.