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

studying a valve case

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

Like Tree3Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   July 30, 2013, 11:55
Default studying a valve case
  #1
New Member
 
Basta
Join Date: Jul 2013
Posts: 28
Rep Power: 4
mina.basta is on a distinguished road
Hi all,

I'm studing a simple case which is a box with circular inlet (velocity 5,3 m/s) and an outlet (pressure =0) with walls and a valve (which is also wall). I simulate with air and using simpleFoam. Attached the pictures of the geometry and in the next post i will attach the problem pictures.
Attached Images
File Type: jpg geometry.jpg (22.6 KB, 52 views)
File Type: jpg valve_pressure.jpg (73.1 KB, 46 views)
File Type: jpg valve_velocity.jpg (39.7 KB, 38 views)
File Type: jpg inlet.jpg (32.1 KB, 34 views)
File Type: jpg inlet_&_outlet.jpg (68.6 KB, 37 views)

Last edited by mina.basta; July 31, 2013 at 03:03.
mina.basta is offline   Reply With Quote

Old   July 30, 2013, 12:00
Default
  #2
New Member
 
Basta
Join Date: Jul 2013
Posts: 28
Rep Power: 4
mina.basta is on a distinguished road
My problem is that using internal field, I have elements with high pressure at the interface between the inlet and the wall. Taking in consideration that I use feature edge: P { margin-bottom: 0.21cm; }
surfaceFeatureExtract -includedAngle 150 -writeObj constant/triSurface/surfacemesh.stl surfacemesh.



Can anybody help me to solve this issue?
Attached Images
File Type: jpg wall.jpg (32.4 KB, 39 views)
File Type: jpg problem_1.jpg (33.6 KB, 32 views)
File Type: jpg problem_2.jpg (29.9 KB, 30 views)
File Type: jpg problem_3.jpg (92.6 KB, 32 views)
File Type: jpg problem_4.jpg (86.8 KB, 29 views)

Last edited by mina.basta; July 31, 2013 at 03:05.
mina.basta is offline   Reply With Quote

Old   July 30, 2013, 15:54
Default
  #3
Senior Member
 
Nima Sam
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,123
Blog Entries: 1
Rep Power: 14
nimasam is on a distinguished road
Send a message via Yahoo to nimasam
it may return to your mesh, first check your mesh with checkMesh
__________________
Training Course on OpenFOAM at (http://www.isme.ir/)
My Weblog (http://openfoam.blogfa.com/)
nimasam is offline   Reply With Quote

Old   July 31, 2013, 02:53
Default
  #4
New Member
 
Basta
Join Date: Jul 2013
Posts: 28
Rep Power: 4
mina.basta is on a distinguished road
Dear Nima Sam,

I already check the mesh, & I think there is no problem.
Code:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create polyMesh for time = 0

Time = 0

Mesh stats
    points:           2025033
    faces:            5508958
    internal faces:   5238048
    cells:            1745217
    boundary patches: 10
    point zones:      0
    face zones:       0
    cell zones:       0

Overall number of cells of each type:
    hexahedra:     1600537
    prisms:        35555
    wedges:        0
    pyramids:      0
    tet wedges:    156
    tetrahedra:    0
    polyhedra:     108969

Checking topology...
    Boundary definition OK.
    Cell to face addressing OK.
    Point usage OK.
    Upper triangular ordering OK.
    Face vertices OK.
    Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces ...
    Patch               Faces    Points   Surface topology                  
    maxY                0        0        ok (empty)                        
    minX                0        0        ok (empty)                        
    maxX                0        0        ok (empty)                        
    minY                0        0        ok (empty)                        
    minZ                0        0        ok (empty)                        
    maxZ                0        0        ok (empty)                        
    stlSurface_entree   9843     10629    ok (non-closed singly connected)  
    stlSurface_mur      181055   187697   ok (non-closed singly connected)  
    stlSurface_sortie   24936    26265    ok (non-closed singly connected)  
    stlSurface_clapet   55076    55667    ok (non-closed singly connected)  

Checking geometry...
    Overall domain bounding box (-0.100007 -0.075 -0.000115936) (0.100007 0.075 0.280004)
    Mesh (non-empty, non-wedge) directions (1 1 1)
    Mesh (non-empty) directions (1 1 1)
    Boundary openness (-9.11983e-18 1.11344e-16 -6.07708e-15) OK.
    Max cell openness = 3.10437e-16 OK.
    Max aspect ratio = 6.2745 OK.
    Minumum face area = 1.68613e-08. Maximum face area = 0.000203991.  Face area magnitudes OK.
    Min volume = 1.03964e-11. Max volume = 2.89671e-06.  Total volume = 0.00758435.  Cell volumes OK.
    Mesh non-orthogonality Max: 51.5309 average: 7.30086
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 3.39272 OK.
    Coupled point location match (average 0) OK.

Mesh OK.

End

Last edited by mina.basta; August 23, 2013 at 04:55.
mina.basta is offline   Reply With Quote

Old   July 31, 2013, 04:35
Default
  #5
Senior Member
 
Nima Sam
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,123
Blog Entries: 1
Rep Power: 14
nimasam is on a distinguished road
Send a message via Yahoo to nimasam
well, did you consider uniform velocity at inlet and fixedValue for walls ?
if yes, you may want to try a profile for inlet velocity to make it much smooth near wall
However you should provide more details until we can help you
__________________
Training Course on OpenFOAM at (http://www.isme.ir/)
My Weblog (http://openfoam.blogfa.com/)
nimasam is offline   Reply With Quote

Old   July 31, 2013, 05:19
Default
  #6
New Member
 
Basta
Join Date: Jul 2013
Posts: 28
Rep Power: 4
mina.basta is on a distinguished road
Dear Nima Sam,

yes I consider uniform velocity with fixedValue at inlet (0 0 5.3) and a fixed value wich is also uniform of (0 0 0) at walls

attached are the U, P, boundary files.

taking in consideration that:
stlSurface_mur --> wall
stlSurface_clapet --> valve
stlSurface_entree ---> inlet
stlSurface_sortie --->outlet

best regards,
Mina
Attached Files
File Type: txt U.txt (1.4 KB, 6 views)
File Type: txt p.txt (1.3 KB, 3 views)
File Type: txt boundary.txt (2.0 KB, 3 views)
File Type: txt blockMeshDict.txt (1.6 KB, 8 views)
mina.basta is offline   Reply With Quote

Old   July 31, 2013, 08:50
Default
  #7
Senior Member
 
Nima Sam
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,123
Blog Entries: 1
Rep Power: 14
nimasam is on a distinguished road
Send a message via Yahoo to nimasam
well, its some how reasonable , you assign a uniform fixed value velocity for inlet and also you assigned a no slip condition on wall ,consider just cells in edges, on those cells should be imposed both above conditions , or in other words when fluid enters geometry with a uniform velocity, it should be compatible with no slip conditions on wall, so it should become zero so in one or two inlet cells you observed a high-pressure as i said in previous post you can assign a non-uniform velocity at inlet, for example parabolic one, then you would not see those high pressure
Paebin likes this.
__________________
Training Course on OpenFOAM at (http://www.isme.ir/)
My Weblog (http://openfoam.blogfa.com/)
nimasam is offline   Reply With Quote

Old   July 31, 2013, 09:04
Default
  #8
New Member
 
Basta
Join Date: Jul 2013
Posts: 28
Rep Power: 4
mina.basta is on a distinguished road
I see, thanks a lot NimaSam for your help i will try now to search about non uniform velocity at inlet.

Regards,
Mina

Quote:
Originally Posted by nimasam View Post
well, its some how reasonable , you assign a uniform fixed value velocity for inlet and also you assigned a no slip condition on wall ,consider just cells in edges, on those cells should be imposed both above conditions , or in other words when fluid enters geometry with a uniform velocity, it should be compatible with no slip conditions on wall, so it should become zero so in one or two inlet cells you observed a high-pressure as i said in previous post you can assign a non-uniform velocity at inlet, for example parabolic one, then you would not see those high pressure
mina.basta is offline   Reply With Quote

Old   July 31, 2013, 09:20
Default
  #9
New Member
 
Basta
Join Date: Jul 2013
Posts: 28
Rep Power: 4
mina.basta is on a distinguished road
But when i tried another geometry for inlet for example a rectangular surface instead of circular one.. I didn't realize these strange elements with high pressure !!!
mina.basta is offline   Reply With Quote

Old   August 16, 2013, 11:21
Default
  #10
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,507
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Greetings to all!

@Mina: I got your PM some time ago, but only today did I manage to look into this.
I only have a few comments to make:
  • The "blockMeshDict" file seems to be in metres, so I guess that you use transformPoints to change from millimetres to metres?
  • The images seem to have been taken while the "p" field was shown in vertex mode. In other words, instead of showing the values in the centre of the cells, it's showing the interpolated values on the vertexes of the mesh. Attached are two images that show the differences between the two modes.
    • The reason why this is important is because the representation you've shown us does not reflect properly where the crazy results are exactly.
    • In addition, you have not indicated what residual values you have for the respective runs, since it's very possible that the first case with the circular inlet didn't converge.
  • Another thing that might help is to use the filters "Slice" and "Extract Cells By Region", which can help you inspect which exact cells have the strange values.
Best regards,
Bruno


edit: Looks like the untrained readers are not able to understand which is which, in the attached images. It's simple:
  • The picture on the left is the one with the cells/faces representation, as you can see from the large data squares in the main 3D display.
  • The picture on the right is the one with the point/vertex/interpolated representation, which is looks so smooth, pretty and not very accurate
Attached Images
File Type: jpg Screenshot from 2013-08-16 16:15:08.jpg (60.7 KB, 37 views)
File Type: jpg Screenshot from 2013-08-16 16:15:02.jpg (57.2 KB, 37 views)

Last edited by wyldckat; August 22, 2013 at 07:29. Reason: see "edit:"
wyldckat is offline   Reply With Quote

Old   August 18, 2013, 13:15
Default
  #11
Senior Member
 
immortality's Avatar
 
Ehsan
Join Date: Oct 2012
Location: Iran
Posts: 2,205
Rep Power: 17
immortality is on a distinguished road
for more clarification,
Quote:
The picture on the right is the one with the point/vertex/interpolated representation, which is looks so smooth, pretty and not very accurate
whats differences between point and vertex?by poit it means its a cell center point and vertices are its corners points,right?
__________________
Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King.
To Be or Not To Be,Thats the Question!
The Only Stupid Question Is the One that Goes Unasked.
immortality is offline   Reply With Quote

Old   August 18, 2013, 13:35
Default
  #12
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,507
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Hi Ehsan,

Quote:
Originally Posted by immortality View Post
whats differences between point and vertex?by poit it means its a cell center point and vertices are its corners points,right?
For reference, the official guide says this: http://www.paraview.org/Wiki/ParaVie...s.2C_arrays.29

I can't believe I'm going to have to explain this ... OK, in ParaView there are three basic geometrical types of representation:
  • Points
  • Lines
  • Surfaces
If this wasn't enough, there are at least two basic types of data content:
  • Data that is registered in points, aka "Point Data". Among these are the following usual usage scenarios:
    • The data is associated to the vertexes of cells and faces as real data.
    • The data is associated to the vertexes of cells and faces as interpolated data. One example of this type of data is to use the filter "Cell Data" to "Point Data".
  • Data that is registered in surfaces, aka "Cell Data". Among these are the following usual usage scenarios:
    • The data is associated to the centre of each cell or face as real data (this is how OpenFOAM usually stores the real data).
    • The data is associated to the centre of each cell or face as interpolated data or perhaps as an average of the data. Example of interpolation for this case is the filter "Cell Data" to "Point Data".
In addition, ParaView uses the following convention:
  • Data on surfaces are either the real values from the centres i.e. "Cell Data" or are showing the interpolated values from the "Point Data".
  • Data on points are usually only the data from themselves, assuming that they have the geometrical characteristic associated to it.
    • Note: Glyphs themselves (e.g. used as vector representation or for seeing where the points are) only work on "Point Data".
  • Data on Lines... are probably what ParaView thinks it's best to show, depending on "Cell Data" or "Point Data".


Is it clear enough now?


Best regards,
Bruno
linnemann and immortality like this.
wyldckat is offline   Reply With Quote

Old   August 18, 2013, 15:54
Default
  #13
Senior Member
 
immortality's Avatar
 
Ehsan
Join Date: Oct 2012
Location: Iran
Posts: 2,205
Rep Power: 17
immortality is on a distinguished road
very good description dear Bruno.there is one cfd-online and one Bruno Santos!
I don't know what I could do if you were not here.
another non related question! how do you write lists in your posts?
__________________
Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King.
To Be or Not To Be,Thats the Question!
The Only Stupid Question Is the One that Goes Unasked.
immortality is offline   Reply With Quote

Old   August 18, 2013, 17:07
Default
  #14
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,507
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Quote:
Originally Posted by immortality View Post
another non related question! how do you write lists in your posts?
Ask here: http://www.cfd-online.com/Forums/sit...k-discussions/
wyldckat is offline   Reply With Quote

Old   August 19, 2013, 06:01
Default
  #15
New Member
 
Basta
Join Date: Jul 2013
Posts: 28
Rep Power: 4
mina.basta is on a distinguished road
Quote:
Originally Posted by wyldckat View Post
Greetings to all!

@Mina: I got your PM some time ago, but only today did I manage to look into this.
I only have a few comments to make:
Dear Bruno,
First of all, my STL file was in "mm" so after blockMesh and snappyhexMesh, I use transfomPoints to change from millimetres to metres. Is there any problems related to this?

Here are some pictures using cells/faces representation

I used these residuals values residualControl
{
p 1e-2;
U 1e-3;
"(k|epsilon|omega)" 1e-3;
}
and I put the endTime in controlDIct file to 3000 but in fact the solution didn't converge and it stops while attending the 3000 and it didn't converge before. I think i can't make the endTime more than 3000 because it took a lot of time to calculate.


and in the next post i will attach other pictures using slice fliter

Regards,
Mina
Attached Images
File Type: jpg Capture1.jpg (43.2 KB, 10 views)
File Type: jpg capture2.jpg (40.1 KB, 7 views)
File Type: jpg capture3.jpg (41.3 KB, 5 views)
File Type: jpg capture4.jpg (40.8 KB, 5 views)
File Type: jpg capture7.jpg (43.5 KB, 2 views)
mina.basta is offline   Reply With Quote

Old   August 19, 2013, 06:02
Default
  #16
New Member
 
Basta
Join Date: Jul 2013
Posts: 28
Rep Power: 4
mina.basta is on a distinguished road
These are other pictures, you can see these strange cells with high pressure .
Attached Images
File Type: jpg capture_slice.jpg (41.9 KB, 20 views)
File Type: jpg capture_slice 2.jpg (80.8 KB, 15 views)
mina.basta is offline   Reply With Quote

Old   August 22, 2013, 07:42
Default
  #17
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,507
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Hi Mina,

OK, there are several issues that seem to be possibly be occurring here:
  1. The cells near the corners of the cylinders are clearly a headache. Having one layer of cells with very low pressure and the ones next to it with high pressure values, seems to indicate that you have got vortexes in the zone of those cells. Here are a few solutions:
    • Remove completely the sharp edge where you're having problems, by applying a fillet in the CAD stage or something. This is if only you can modify the geometry.
    • Increase or reduce the mesh resolution near the edges of that cylinder, so that it can either better solve the vortexes or completely ignore them.
  2. It all depends if you have the turbulence model turned on or off. Because if you are solving in laminar mode, you will need very low inlet and outlet fluid speeds.
  3. If you are using a turbulence model, then you should check the y+ "yPlus" field on the walls. You can run:
    Code:
    yPlusRAS
    to calculate the y+.
    Depending on the values you get for y+, you need to adjust your mesh accordingly. More on this topic: http://www.cfd-online.com/Wiki/Dimen...e_%28y_plus%29


Best regards,
Bruno
wyldckat is offline   Reply With Quote

Old   August 22, 2013, 11:45
Default
  #18
New Member
 
Basta
Join Date: Jul 2013
Posts: 28
Rep Power: 4
mina.basta is on a distinguished road
Quote:
Originally Posted by wyldckat View Post
Hi Mina,

OK, there are several issues that seem to be possibly be occurring here:
  1. The cells near the corners of the cylinders are clearly a headache. Having one layer of cells with very low pressure and the ones next to it with high pressure values, seems to indicate that you have got vortexes in the zone of those cells. Here are a few solutions:
Dear Bruno,

Thank you so much for your reply.
I created a very simple case which is a simple cylinder with inlet (velocity =5.3), walls , outlet (P=0).
I used the solver simpleFoam with turbulent.
I tried to vary the mesh with different values, increasing and reducing also i tried to apply a filled but the same problem is still there.
I'm so surprise, I attached some pictures which explain this issue.
Attached Images
File Type: jpg capture1.jpg (42.1 KB, 22 views)
File Type: jpg capture 2.jpg (51.4 KB, 14 views)
File Type: jpg capture2-.jpg (54.3 KB, 14 views)
File Type: jpg capture3.jpg (99.6 KB, 15 views)
File Type: jpg capture4.jpg (46.4 KB, 10 views)

Last edited by mina.basta; August 23, 2013 at 04:37.
mina.basta is offline   Reply With Quote

Old   August 23, 2013, 04:25
Default
  #19
Member
 
Martin Novák
Join Date: Dec 2012
Location: Prague
Posts: 56
Rep Power: 4
novakm is on a distinguished road
Quote:
Originally Posted by mina.basta View Post
Dear Bruno,

Thank you so much for your reply.
I created a very simple case which is a simple cylinder with inlet (velocity =5.3), walls , outlet (P=0).
I used the solver simpleFoam zith turbulent.
I tried to vary the mesh with different values, increasing and reducing also i tried to apply a filled but the same problem is still there.
I'm so surprise, I attached some pictures which explain this issue.
Hi Mina.

Could you post here the test case?
This is strange behavior indeed
I am guessing that it is caused due an inconsistent boundary conditions or due the numerical pressure singularity phenomena (e.g."L" problem or squeeze flow issue).

Btw. It is usual to use pressure driven flow. In the test case that can be interpreted as PRESSURE driven flow in cylindrical pipe there exists an analytical solution. You can find it as Poiseuille fluid flow. It could help you to set the model properly.

Best regards

Martin
novakm is offline   Reply With Quote

Old   August 23, 2013, 04:47
Default
  #20
New Member
 
Basta
Join Date: Jul 2013
Posts: 28
Rep Power: 4
mina.basta is on a distinguished road
Quote:
Originally Posted by novakm View Post
Hi Mina.

Could you post here the test case?
Dear Martin,

here is the test case
Attached Files
File Type: gz test case.tar.gz (2.1 KB, 6 views)
mina.basta is offline   Reply With Quote

Reply

Tags
nimasam

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
Valve simulation with spring - FSI? Help! farianka CFX 1 April 17, 2011 18:04
Simulation of air flow inside valve - FSI? Help! farianka Main CFD Forum 0 April 17, 2011 16:30
Ansys FSI and CFX (valve simulation) farianka ANSYS 0 April 17, 2011 16:20
Terrible Mistake In Fluid Dynamics History Abhi Main CFD Forum 12 July 8, 2002 09:11
Valve Forces in CFdesign Mike Clapp Main CFD Forum 3 March 8, 2001 15:09


All times are GMT -4. The time now is 08:32.