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

Gravitational water flow in closed channel.

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 28, 2013, 08:11
Default Gravitational water flow in closed channel.
  #1
New Member
 
Szymon
Join Date: Aug 2013
Posts: 4
Rep Power: 4
Szymon85 is on a distinguished road
Hello everyone,

I have a problem with the modeling of two-phase flow in the channel as shown in the figure. Fluid intake is at the top of the channel and the outlet at the bottom (Z axis is vertical). One phase is water with a given volume flow rate, flowing down the channel. The second phase is the air moving freely. Everything is carried out under atmospheric pressure. I have very little experience in the use of CFD software, so I tried to use the tutorial "Free Surface Flow Over a Bump". I decided that this example is similar to my problem. But my case differs from that of the tutorial in the following way:
- Movement in 3D, rather than 2D;
- Flow of water under the force of gravity.


I loaded Bump2D.pre, deleted the tutorial model and loaded the mine. I removed the unnecessary borders leaving "inflow", "outflow" and "wall". Also introduced another change in one equation by adding value 85000Pa: DenH*g*DownVFWater*(DownH-y)+85000 [Pa]. Additional 85000 Pa to the pressure at the outlet of the channel is derived from the hydrostatic pressure of water, arising from the difference of levels (ca. 9 meters) between the inlet and the outlet.

Unfortunately, results are unsatisfactory. Streamline velocity of the water does not reach the outlet of the channel only breaks along the way. I started to change various parameters, creat flow pattern from beginning. I tried to change geometry, the boundaries, transient calculation. All of my efforts were to no avail. I received results similar to that described above or completely meaningless.
I was looking for some clues to topics in this forum and on the Internet, but it did not help. So I ask for some help, maybe another tutorial? What is wrong?


channel.png
Szymon85 is offline   Reply With Quote

Old   August 28, 2013, 18:18
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,937
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Can you show an image of what you are getting, and some pictures of your mesh.
ghorrocks is offline   Reply With Quote

Old   August 29, 2013, 06:34
Default
  #3
New Member
 
Szymon
Join Date: Aug 2013
Posts: 4
Rep Power: 4
Szymon85 is on a distinguished road
Picture of the mesh:

In mesh generator I choose:
“Defaults”:
- “Physics Preference” – “CFD”
- “Solver Preference” – “CFX”
“Sizing”:
- “Relevance Center” – “Medium”
Other options I left untouched.

Picture of the results:
Szymon85 is offline   Reply With Quote

Old   August 29, 2013, 06:58
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,937
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
The problem is obvious - your mesh is far too coarse and the water is getting diffused away. You need a finer mesh across the section (but you mesh along the length is OK for starters). Once you have got the water flowing the full length of the pipe then you will need to do a sensitivity analysis on the section and length mesh resolution to get an accurate simulation.
ghorrocks is offline   Reply With Quote

Old   August 30, 2013, 10:09
Default
  #5
New Member
 
Szymon
Join Date: Aug 2013
Posts: 4
Rep Power: 4
Szymon85 is on a distinguished road
Thanks for answer ghorrocks,
But I have antoher problem. Following your advice I thickened mesh by setting options: "Max face size" and "Max size" to 0,025m. Next I run calculations and recive error:
Quote:
+--------------------------------------------------------------------+
| Mesh Statistics |
+--------------------------------------------------------------------+
| Domain Name | Orthog. Angle | Exp. Factor | Aspect Ratio |
+----------------------+---------------+--------------+--------------+
| | Minimum [deg] | Maximum | Maximum |
+----------------------+---------------+--------------+--------------+
| Default Domain | 30.0 ok | 38 ! | 10 OK |
+----------------------+---------------+--------------+--------------+
| | %! %ok %OK | %! %ok %OK | %! %ok %OK |
+----------------------+---------------+--------------+--------------+
| Default Domain | 0 <1 100 | <1 <1 100 | 0 0 100 |
+----------------------+---------------+--------------+--------------+

Domain Name : Default Domain

Total Number of Nodes = 9576223

Total Number of Elements = 9914285
Total Number of Tetrahedrons = 198844
Total Number of Prisms = 13346
Total Number of Hexahedrons = 9125695
Total Number of Pyramids = 576400

Total Number of Faces = 399964

+--------------------------------------------------------------------+
| Buoyancy Reference Information |
+--------------------------------------------------------------------+

Domain Group: Default Domain

Buoyancy has been activated. The absolute pressure will include
hydrostatic pressure contribution, using the following reference
coordinates: (-7.24678E+00,-1.61470E+01, 2.70001E+00).

+--------------------------------------------------------------------+
| Checking for Isolated Fluid Regions |
+--------------------------------------------------------------------+

No isolated fluid regions were found.

CFD Solver started: Fri Aug 30 13:54:53 2013


+--------------------------------------------------------------------+
| Convergence History |
+--------------------------------------------------------------------+

================================================== ====================
| Timescale Information |
----------------------------------------------------------------------
| Equation | Type | Timescale |
+----------------------+------------------------+--------------------+
| U-Mom-Bulk | Physical Timescale | 2.50000E-01 |
| V-Mom-Bulk | Physical Timescale | 2.50000E-01 |
| W-Mom-Bulk | Physical Timescale | 2.50000E-01 |
| Mass-Water | Physical Timescale | 2.50000E-01 |
| Mass-Air | Physical Timescale | 2.50000E-01 |
+----------------------+------------------------+--------------------+
+----------------------+------------------------+--------------------+
| K-TurbKE-Bulk | Physical Timescale | 2.50000E-01 |
| E-Diss.K-Bulk | Physical Timescale | 2.50000E-01 |
+----------------------+------------------------+--------------------+

================================================== ====================
OUTER LOOP ITERATION = 3 ( 1) CPU SECONDS = 1.016E+03 (1.910E+02)
----------------------------------------------------------------------
| Equation | Rate | RMS Res | Max Res | Linear Solution |
+----------------------+------+---------+---------+------------------+

+--------------------------------------------------------------------+
| *** INSUFFICIENT MEMORY ALLOCATED *** |
| |
| ACTION REQUIRED : Increase the real stack memory size. |
| |
| Details : |
| Requested space : 1735841844 words |
| Current allocated space : 2147483646 words |
| Current used space : 1055776224 words |
| Current free space : 1091707422 words |
| Number of free areas : 1 |
+--------------------------------------------------------------------+


Details of error:-
----------------
Error detected by routine MAKDAT
CDANAM = A CDTYPE = REAL ISIZE = 1735841844
CRESLT = FULL

Current Directory : /FLOW/SOLVER/TIME-0/HYDRO_SS1

+--------------------------------------------------------------------+
| Writing crash recovery file |
+--------------------------------------------------------------------+

Details of error:-
----------------
Error detected by routine POPDIR
CRESLT = ILEG

Current Directory : /FLOW/NAMEMAP

+--------------------------------------------------------------------+
| An error has occurred in cfx5solve: |
| |
| The ANSYS CFX solver exited with return code 1. No results file |
| has been created. |
+--------------------------------------------------------------------+

End of solution stage.

+--------------------------------------------------------------------+
| Warning! |
| |
| The ANSYS CFX Solver has written a crash recovery file. This file |
| has been saved as C:/rura |
| siatka_pending_tasks/dp0_CFX_Solution/Bump2D_001.res.err and may |
| be an aid to diagnosing the problem or restarting the run. More |
| details should be available in the solver output section of the |
| output file. |
+--------------------------------------------------------------------+


+--------------------------------------------------------------------+
| Warning! |
| |
| After waiting for 60 seconds, 1 solver manager process(es) appear |
| not to have noticed that this run has ended. You may get errors |
| removing some files if they are still open in the solver manager. |
+--------------------------------------------------------------------+


This run of the ANSYS CFX Solver has finished.
I've checked that error in google. Before run calculations I changed in solver tab value of "Memory Alloc Factor" to 1.3x, next time to 2x. Itdidn't work, so I try enter a specific value in "Detailed Memory Overrides" -> "Real Memory" -> <1800m>, because cfx request for space: 1735841844 words. After that I received error again.
I read that can be connected with mesh or setup errors, but before I refined the mesh I recived some results. Obviously that results were wrong, but simulations run from start to end without errors. Maybe the mesh is too small?
Szymon85 is offline   Reply With Quote

Old   August 30, 2013, 21:55
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,937
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
You have run out of RAM on the PC you are running on. Either make the simulation smaller (but this requires some skill to make it smaller and still retain the essential detail), install more memory or do a multi-processor run.
ghorrocks is offline   Reply With Quote

Old   September 3, 2013, 03:02
Default
  #7
New Member
 
Szymon
Join Date: Aug 2013
Posts: 4
Rep Power: 4
Szymon85 is on a distinguished road
Hello everybody, especially ghorrocks,

I have questions, again J. I’ve made smaller simulation, like ghorrocks advised me. I changed min size of mesh to 0,05m. I also noticed that I had wrong variable in expressions in CFX-pre. In tutorial vertical axis is Y, in my simulation vertical is Z.So I changed it.


I run calculations which was ended without error and without warning about artificial wall at the outlet. So I thought everything is OK, but unfortunately not. Streamlines of water and air velocity looks like flow mixed, but should be separate. I also expected higher water velocity. Now, I don’t know what could be wrong, I have no idea. Earlier I have these streamlines separate. Below I put some simulation setup and streamlines of water and air.



















Szymon85 is offline   Reply With Quote

Old   September 3, 2013, 16:28
Default
  #8
Senior Member
 
Bruno
Join Date: Mar 2009
Location: Brazil
Posts: 236
Rep Power: 12
brunoc is on a distinguished road
Phase.Velocity is calculated for the entire domain, regardless of whether the local volume fraction is 0 or 1. You want to plot the values for Superficial Velocity, which is volume_fraction * velocity.

To just look at the air-water interface, create an isosurface of Water.Volume Fraction = 0.5.

About your mesh, you need to refine it only near the wall. Check the meshing tutorials about 'Inflation'.
brunoc is offline   Reply With Quote

Reply

Tags
cfx, gravitational flow, water and air

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
free surface flow inside channel that gets narrower JohnAB STAR-CCM+ 4 June 24, 2013 15:48
Mass Flow rate in spray water modeling Behnam Ghadimi FLUENT 0 June 8, 2013 16:05
Mass Flow rate in spray water modeling Behnam Ghadimi Main CFD Forum 0 June 8, 2013 15:48
Pressure outlet in two-phase flow in horizontal 2D channel AlmostSurelyRob Main CFD Forum 0 November 17, 2010 08:32
uptodate water distribution network fredius,magige,tanzanian,(e.a) Main CFD Forum 0 January 27, 2002 08:10


All times are GMT -4. The time now is 12:34.