|
[Sponsors] |
July 30, 2013, 11:55 |
studying a valve case
|
#1 |
New Member
Basta
Join Date: Jul 2013
Posts: 28
Rep Power: 13 |
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. Last edited by mina.basta; July 31, 2013 at 03:03. |
|
July 30, 2013, 12:00 |
|
#2 |
New Member
Basta
Join Date: Jul 2013
Posts: 28
Rep Power: 13 |
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? Last edited by mina.basta; July 31, 2013 at 03:05. |
|
July 30, 2013, 15:54 |
|
#3 |
Senior Member
Nima Samkhaniani
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,266
Blog Entries: 1
Rep Power: 25 |
it may return to your mesh, first check your mesh with checkMesh
__________________
My Personal Website (http://nimasamkhaniani.ir/) Telegram channel (https://t.me/cfd_foam) |
|
July 31, 2013, 02:53 |
|
#4 |
New Member
Basta
Join Date: Jul 2013
Posts: 28
Rep Power: 13 |
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. |
|
July 31, 2013, 04:35 |
|
#5 |
Senior Member
Nima Samkhaniani
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,266
Blog Entries: 1
Rep Power: 25 |
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
__________________
My Personal Website (http://nimasamkhaniani.ir/) Telegram channel (https://t.me/cfd_foam) |
|
July 31, 2013, 05:19 |
|
#6 |
New Member
Basta
Join Date: Jul 2013
Posts: 28
Rep Power: 13 |
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 |
|
July 31, 2013, 08:50 |
|
#7 |
Senior Member
Nima Samkhaniani
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,266
Blog Entries: 1
Rep Power: 25 |
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
__________________
My Personal Website (http://nimasamkhaniani.ir/) Telegram channel (https://t.me/cfd_foam) |
|
July 31, 2013, 09:04 |
|
#8 | |
New Member
Basta
Join Date: Jul 2013
Posts: 28
Rep Power: 13 |
I see, thanks a lot NimaSam for your help i will try now to search about non uniform velocity at inlet.
Regards, Mina Quote:
|
||
July 31, 2013, 09:20 |
|
#9 |
New Member
Basta
Join Date: Jul 2013
Posts: 28
Rep Power: 13 |
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 !!!
|
|
August 16, 2013, 11:21 |
|
#10 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,980
Blog Entries: 45
Rep Power: 128 |
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:
Bruno edit: Looks like the untrained readers are not able to understand which is which, in the attached images. It's simple:
__________________
Last edited by wyldckat; August 22, 2013 at 07:29. Reason: see "edit:" |
|
August 18, 2013, 13:15 |
|
#11 | |
Senior Member
Ehsan
Join Date: Oct 2012
Location: Iran
Posts: 2,208
Rep Power: 27 |
for more clarification,
Quote:
__________________
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. |
||
August 18, 2013, 13:35 |
|
#12 | |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,980
Blog Entries: 45
Rep Power: 128 |
Hi Ehsan,
Quote:
I can't believe I'm going to have to explain this ... OK, in ParaView there are three basic geometrical types of representation:
Is it clear enough now? Best regards, Bruno
__________________
|
||
August 18, 2013, 15:54 |
|
#13 |
Senior Member
Ehsan
Join Date: Oct 2012
Location: Iran
Posts: 2,208
Rep Power: 27 |
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. |
|
August 18, 2013, 17:07 |
|
#14 | |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,980
Blog Entries: 45
Rep Power: 128 |
Quote:
|
||
August 19, 2013, 06:01 |
|
#15 | |
New Member
Basta
Join Date: Jul 2013
Posts: 28
Rep Power: 13 |
Quote:
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 |
||
August 19, 2013, 06:02 |
|
#16 |
New Member
Basta
Join Date: Jul 2013
Posts: 28
Rep Power: 13 |
These are other pictures, you can see these strange cells with high pressure .
|
|
August 22, 2013, 07:42 |
|
#17 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,980
Blog Entries: 45
Rep Power: 128 |
Hi Mina,
OK, there are several issues that seem to be possibly be occurring here:
Best regards, Bruno
__________________
|
|
August 22, 2013, 11:45 |
|
#18 | |
New Member
Basta
Join Date: Jul 2013
Posts: 28
Rep Power: 13 |
Quote:
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. Last edited by mina.basta; August 23, 2013 at 04:37. |
||
August 23, 2013, 04:25 |
|
#19 | |
Member
Martin Novák
Join Date: Dec 2012
Location: Prague
Posts: 70
Rep Power: 13 |
Quote:
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 |
||
August 23, 2013, 04:47 |
|
#20 |
New Member
Basta
Join Date: Jul 2013
Posts: 28
Rep Power: 13 |
Dear Martin,
here is the test case |
|
Tags |
nimasam |
Thread Tools | Search this Thread |
Display Modes | |
|
|
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 14:09 |