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

Axisymmetric Flow: Incorrect Pressure at Axis and Sudden Pressure Drop at Outlet BC

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 26, 2020, 19:53
Default Axisymmetric Flow: Incorrect Pressure at Axis and Sudden Pressure Drop at Outlet BC
  #1
Member
 
CWL
Join Date: Nov 2015
Posts: 56
Rep Power: 7
cwl6750084 is on a distinguished road
I appreciate if any person can offer some ideas on the following issues?

I am running an axisymmetric simulations of a nozzle. However, the pressure along a large portion of the axis is always equals to the value I set at the outlet boundary. Does anyone knows how to solve the problem? In particular, the pressure value of the outlet (to the right of the figure) is 2.5 MPa, the inlet pressure is 10 MPa.

Moreover, for some reasons, the values of pressure on the nodes immediately before the outlet BC at much higher (at about 9 MPa), then, it suddenly drops to the boundary value in only a distance of one mesh cell. Does this have anything to do with the weird pressure distribution on the axis? Any idea how to correct these issues?
Attached Images
File Type: jpg Pressure on Axis.jpg (30.1 KB, 15 views)
File Type: jpg Pressure vs x.jpg (42.9 KB, 9 views)
cwl6750084 is offline   Reply With Quote

Old   March 27, 2020, 04:27
Default Axis Boundary
  #2
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,948
Blog Entries: 1
Rep Power: 32
vinerm will become famous soon enough
Could you confirm if axis is really defined as axis type under boundary condition? It should not be defined as any other type. Furthermore, it should really be aligned with the x-axis to behave like an axis. This is not a requirement for axisymmetric scenario, such as, an annulus, but for the cases that have their domain touching the axis.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   March 27, 2020, 18:14
Default
  #3
Member
 
CWL
Join Date: Nov 2015
Posts: 56
Rep Power: 7
cwl6750084 is on a distinguished road
Hi,

Thanks for your reply.

Yes, the axis is defined using the axis type and perfectly aligned along the x-axis. There are no nodes lying below the x-axis.

When I plot the pressure contour using cell values, the pressure-field looks continuous. I do not understand the discrepancy. Should the contours from both not be the same? When should I look at node values versus cell values.

Do you think this is related with the suddenly drop of pressure (other other flow variables) at the outlet boundary?
Attached Images
File Type: jpg Mesh.jpg (121.2 KB, 13 views)
cwl6750084 is offline   Reply With Quote

Old   March 28, 2020, 16:46
Default Node values
  #4
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,948
Blog Entries: 1
Rep Power: 32
vinerm will become famous soon enough
Fluent calculates everything at cell centers. Values at the nodes are interpolated using gradients. Therefore, there is always a difference. However, that cannot explain what you observed.

Though the details of the mesh show minimum y as 0.0, still why are there two lines near the axis in the image you shared? Or it could be just visual.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   March 28, 2020, 16:57
Default
  #5
Member
 
CWL
Join Date: Nov 2015
Posts: 56
Rep Power: 7
cwl6750084 is on a distinguished road
The two lines should be just the resolution. For some reason the image downloaded from here looks kind of blur when zoomed in.

I actually exported the ASCII data file and the minimum y-coordinate for each given x-coordinate are actually 0.00000. There are no nodes below the x-axis.
cwl6750084 is offline   Reply With Quote

Old   March 28, 2020, 17:08
Default Node on negative y
  #6
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,948
Blog Entries: 1
Rep Power: 32
vinerm will become famous soon enough
That's good. Fluent does not run if it detects even a single node on negative y. However, it is not must to have any element lying on x-axis. E.g., if the geometry represents annular region, all nodes will have y > 0 and none with y=0.

Is the solution properly converged then? And if you plot y-velocity, does it show any negative velocity near the axis? As per the pressure field, it should show that. That implies the solution is not fully converged. If that is the case, try using some other numerical scheme.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   March 30, 2020, 18:59
Default
  #7
Member
 
CWL
Join Date: Nov 2015
Posts: 56
Rep Power: 7
cwl6750084 is on a distinguished road
Hello,

Based on the residual curves, they are all at least 3 orders of magnitude smaller than the initial values. Moreover, when I checked the averaged values at the nozzle exit (the second vertical line from the right in the mesh), they are pretty constant even I ran the simulation for 800000 iterations. That is why I am not sure that this is an issue with not sufficiently converged.

Per you suggestions, it seems that there is slight negative radial velocity at the beginning of the nozzle. But that does not correspond the region where P_axis = P_out.

Is there a general rule on Node Values versus Cell Values. The simulation is about liquid water being evaporated to water vapour. I am treating the vapour as ideal gas as the real gas law does not work.

I am using Coupled scheme with 2nd order Upwind for all variables. This is the only possible scheme for the simulation as anything else would crash.
Attached Images
File Type: jpg Velocity.jpg (33.9 KB, 4 views)
File Type: jpg Convergence.jpg (39.7 KB, 4 views)

Last edited by cwl6750084; March 30, 2020 at 19:01. Reason: Include Figures
cwl6750084 is offline   Reply With Quote

Old   March 31, 2020, 05:04
Default Multiphase
  #8
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,948
Blog Entries: 1
Rep Power: 32
vinerm will become famous soon enough
If the simulation is multiphase, operating conditions will have a lot of effect. Do check the following

1. Value and direction of gravity. It must be either -9.81 or 9.81 in x-direction. Gravity cannot be in y-direction for axisymmetric case.

2. Reference location for the operating pressure should be the highest point in the domain. If gravity is -9.81, then maximum value of x in the domain should be used as reference location and vice-versa.

3. Operating density should be the density of the gas phase.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   April 3, 2020, 03:56
Default
  #9
Member
 
CWL
Join Date: Nov 2015
Posts: 56
Rep Power: 7
cwl6750084 is on a distinguished road
Quote:
Originally Posted by vinerm View Post
If the simulation is multiphase, operating conditions will have a lot of effect. Do check the following

1. Value and direction of gravity. It must be either -9.81 or 9.81 in x-direction. Gravity cannot be in y-direction for axisymmetric case.

2. Reference location for the operating pressure should be the highest point in the domain. If gravity is -9.81, then maximum value of x in the domain should be used as reference location and vice-versa.

3. Operating density should be the density of the gas phase.
I used 9.81 for gravity in the position x-direction and the minimum value of x (inlet) for operating condition. However, I used 0 for the operating condition per the instruction in Fluent for compressible phase (water vapour). It seems that the pressure field does not match the outlet BC because the domain is not long enough, though I do not know why - as I thought the boundaries are always matched.

However, the nodal pressure along the axis are still very low (almost equals to the outlet pressure and I am not sure what else can alter that).
Attached Images
File Type: jpg Pressure.jpg (35.6 KB, 6 views)
cwl6750084 is offline   Reply With Quote

Old   April 6, 2020, 06:55
Default Operating Conditions
  #10
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,948
Blog Entries: 1
Rep Power: 32
vinerm will become famous soon enough
If you are using ideal or real gas, then operating density as well as operating pressure, both should be set to 0. And the pressure at the outlet should have some positive value.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   April 10, 2020, 22:11
Default
  #11
Member
 
CWL
Join Date: Nov 2015
Posts: 56
Rep Power: 7
cwl6750084 is on a distinguished road
Quote:
Originally Posted by vinerm View Post
If you are using ideal or real gas, then operating density as well as operating pressure, both should be set to 0. And the pressure at the outlet should have some positive value.
Yes, I have been using both as zeroes for both operation density and operation pressure.

The value at the outlet boundary, for some reasons, will not match when I turn on the phase change (evaporation from water to steam). When I run single phase simulation (i.e. without evaporation), the values at both ends match well.

For multiphase calculation, the outlet boundary value will only match if the mesh is very long.

Does Fluent treat single phase and multiphase calculations differently?
Attached Images
File Type: jpg Liquid.jpg (88.9 KB, 8 views)
File Type: jpg Multiphase.jpg (87.3 KB, 9 views)
File Type: jpg Gas.jpg (77.7 KB, 7 views)
cwl6750084 is offline   Reply With Quote

Old   April 11, 2020, 10:17
Default Pressure
  #12
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,948
Blog Entries: 1
Rep Power: 32
vinerm will become famous soon enough
I am sorry, I could not understand what you mean by the statement
Quote:
The value at the outlet boundary, for some reasons, will not match
Which boundaries are you comparing for matching the pressure values?
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   April 27, 2020, 07:53
Default
  #13
Member
 
CWL
Join Date: Nov 2015
Posts: 56
Rep Power: 7
cwl6750084 is on a distinguished road
Quote:
Originally Posted by vinerm View Post
I am sorry, I could not understand what you mean by the statement Which boundaries are you comparing for matching the pressure values?
If you look at the graph for multiphase, the pressure at the right edge of the graph (corresponds to the pressure outlet in the computational domain), the pressures is much higher than the pressure specified at the outlet. When I downloaded the numerical data, the pressure simply dropped from the node right before the outlet boundary to the specified value on the outlet boundary. I do not understand why there is such a discontinuity right before the outler boundary for the multi-phase case.
cwl6750084 is offline   Reply With Quote

Old   April 28, 2020, 08:44
Default
  #14
Senior Member
 
duri
Join Date: May 2010
Posts: 245
Rep Power: 13
duri is on a distinguished road
Quote:
Originally Posted by cwl6750084 View Post
I am running an axisymmetric simulations of a nozzle. However, the pressure along a large portion of the axis is always equals to the value I set at the outlet boundary. Does anyone knows how to solve the problem? In particular, the pressure value of the outlet (to the right of the figure) is 2.5 MPa, the inlet pressure is 10 MPa.

Moreover, for some reasons, the values of pressure on the nodes immediately before the outlet BC at much higher (at about 9 MPa), then, it suddenly drops to the boundary value in only a distance of one mesh cell. Does this have anything to do with the weird pressure distribution on the axis? Any idea how to correct these issues?

Try to plot the cell values which is the actual solution. The sudden drop in pressure and probably the strange pressure distribution in axis may be due to interpolation to node values.

The solution indicate the interior zone is ignorant of exit pressure. It probably means supersonic flow condition exist near the outlet condition. There could be other reasons as well but I couldn't guess from the given information. (Mach number plot, solver settings and boundary condition can help) Typically for a CD nozzle when supersonic flow is reached the outlet boundary condition is transferred through boundary layer which helps to produce over expanded condition. But in this case, the picture shows boundary layer ceases to exist after divergent wall. Try to initialize from subsonic solution.
duri is offline   Reply With Quote

Old   May 4, 2020, 16:15
Default
  #15
Member
 
CWL
Join Date: Nov 2015
Posts: 56
Rep Power: 7
cwl6750084 is on a distinguished road
Quote:
Originally Posted by duri View Post
Try to plot the cell values which is the actual solution. The sudden drop in pressure and probably the strange pressure distribution in axis may be due to interpolation to node values.

The solution indicate the interior zone is ignorant of exit pressure. It probably means supersonic flow condition exist near the outlet condition. There could be other reasons as well but I couldn't guess from the given information. (Mach number plot, solver settings and boundary condition can help) Typically for a CD nozzle when supersonic flow is reached the outlet boundary condition is transferred through boundary layer which helps to produce over expanded condition. But in this case, the picture shows boundary layer ceases to exist after divergent wall. Try to initialize from subsonic solution.
Thank you for the very insightful comment. Actually, the flow should be subsonic throughout the nozzle, the maximum velocity is only 270 m/s and the temperature is over 500 K. The sonic speed for steam is over 500 m/s at that temperature and even higher for liquid water. (I could not figure out how to define the sonic speed for two-phase flow.)

What did you mean by "initialize from subsonic solution"?
cwl6750084 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
Erroneous eddy viscosity ratio for pipe flow preis OpenFOAM Running, Solving & CFD 1 May 11, 2018 20:58
Pressure loss due to sudden expansion in pipe flow Ahmed FLUENT 0 January 2, 2006 11:01


All times are GMT -4. The time now is 05:53.