|
[Sponsors] |
July 5, 2014, 03:35 |
Negative pressure problem
|
#1 |
Member
Ben B. Huang
Join Date: Oct 2012
Posts: 54
Rep Power: 13 |
Hey, guys
I am simulating a simple model(see attached figs). But the results are far from reality. Inlet: opening B.C. with static pressure(the value=rho*g*h where h=60). Outlet: relative pressure=0 Others: wall B.C.. I can not figure out why there is so large negative pressure at the vicinity of branch pipe. I really appreciate your help. |
|
July 5, 2014, 05:59 |
|
#2 |
Senior Member
Blanco
Join Date: Mar 2009
Location: Torino, Italy
Posts: 193
Rep Power: 17 |
Hi,what is the numerical setup? and what about turbulence model, mesh in the branch pipe? you are obtaining 40 m/s maximum velocity in the connection, I think you have boundary layer separation there, that s why you get negative pressure...
|
|
July 5, 2014, 06:46 |
|
#3 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,700
Rep Power: 143 |
The low pressure region is clearly a separation.
I can also see your contour lines are jagged which is a sure sign of your mesh being too coarse. Have you read this FAQ? http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F |
|
July 5, 2014, 06:50 |
|
#4 |
New Member
Join Date: Jan 2014
Posts: 2
Rep Power: 0 |
Dear you dint not supply full information. Its simulation shows that your mesh is unstructured and not adequate. what is your turbulence model? working fluid and reference pressure. Plot Absolute pressure instead of pressure to get a clear picture.
|
|
July 5, 2014, 07:34 |
|
#5 | |
Member
Ben B. Huang
Join Date: Oct 2012
Posts: 54
Rep Power: 13 |
Quote:
k-e model and unstructured mesh. If there is boundary layer separation, what can I do next to fix this? refine mesh elements or something else? |
||
July 5, 2014, 07:49 |
|
#6 | |
Member
Ben B. Huang
Join Date: Oct 2012
Posts: 54
Rep Power: 13 |
Quote:
It is not right because there will be cavitation. How can I improve it or redo the simulation the right way? I really look into that FAQ before and I cannot find out a way. thank you for your help. |
||
July 5, 2014, 08:06 |
|
#7 |
Senior Member
Blanco
Join Date: Mar 2009
Location: Torino, Italy
Posts: 193
Rep Power: 17 |
Ok, yes you have to refine the mesh in the separation zone and just ahead/after it, to improve the definition of the physical domain and so improve the solution. Btw, what is the minimum absolute pressure reached in the separating zone? I suppose negative pressure you talked about was relative pressure, take a look at abs values. You talked also about cavitation, if you expect cavitation than you need to have a model for it.
Regards |
|
July 5, 2014, 08:07 |
|
#8 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,700
Rep Power: 143 |
If you are using a reference pressure of 1 bar and your working fluid is water then you are miles away from cavitation.
And if the simulation is accurate and it predicts a separation - then the system you are modelling has a separation, so your simulation is correct. Or do you know that a separation does not exist? |
|
July 5, 2014, 08:26 |
|
#9 | |
Member
Ben B. Huang
Join Date: Oct 2012
Posts: 54
Rep Power: 13 |
Quote:
In this model, the reference pressure is 1 bar, but I used '9.8 kPa' to plot the pressure contour(see the figure above). The negative pressure is about 55*9.8 kPa(water head=55m if this is right). We have the physical model in fact but cannot observe the flow because that part is inside a wall of the physical model, so we simulate it to see what happens. So I cannot be sure there is separation or not, but I think there is. any suggestions? |
||
July 5, 2014, 08:35 |
|
#10 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,700
Rep Power: 143 |
Well if you are trying to say that the pressure in that region = 101-55*9.8 = -437kPa absolute then it will (almost) definitely cavitate. It appears like you have not run a cavitation model so then all this model tells you is that it cavitates - the actual flow and pressure field it predicts is wrong.
|
|
July 5, 2014, 08:41 |
|
#11 | |
Member
Ben B. Huang
Join Date: Oct 2012
Posts: 54
Rep Power: 13 |
Quote:
|
||
July 5, 2014, 08:48 |
|
#12 | |
Member
Ben B. Huang
Join Date: Oct 2012
Posts: 54
Rep Power: 13 |
Quote:
Thank you so much. |
||
July 5, 2014, 10:51 |
|
#13 |
Senior Member
Blanco
Join Date: Mar 2009
Location: Torino, Italy
Posts: 193
Rep Power: 17 |
Well, if pressure is -437 kPa then it almost definitely cavitate as it has been said. The boundary layer separation will be present also in the real Fluid behavior, if everything is correct in the setup, and it will cause the pressure decrease that lead to cavitation, but if you don t model cavitation you can't refer to the pressure and velocity field obtained...you just know that cavitation will happen there, nothing more.
Last edited by Blanco; July 5, 2014 at 12:19. |
|
July 5, 2014, 12:23 |
|
#14 |
Senior Member
Blanco
Join Date: Mar 2009
Location: Torino, Italy
Posts: 193
Rep Power: 17 |
Wait...just to be sure I understood right...in your plot I see ref. Pressure 9.8 kPa and then -55 Pa in the figure...so you get 9.75 kPa minum absolute pressure, not -437 kPa, is this correct? if this is correct then you simply have to check if cavitation would happen at 9750 Pa
|
|
July 5, 2014, 21:34 |
|
#15 | |
Member
Ben B. Huang
Join Date: Oct 2012
Posts: 54
Rep Power: 13 |
Quote:
I think maybe this cause the confusion. I am going to refine the mesh first and see what will happen. Thank you so much. |
||
July 6, 2014, 00:31 |
|
#16 |
Member
Ben B. Huang
Join Date: Oct 2012
Posts: 54
Rep Power: 13 |
hey there
I refined the mesh and the problem is still there. any suggestions? Thank you in advance. |
|
July 6, 2014, 00:35 |
|
#17 | |
Member
Ben B. Huang
Join Date: Oct 2012
Posts: 54
Rep Power: 13 |
Quote:
any suggestions about the boundary-layer separation? Or is this reasonable? thank you for your time. |
||
July 6, 2014, 03:17 |
|
#18 |
Senior Member
Blanco
Join Date: Mar 2009
Location: Torino, Italy
Posts: 193
Rep Power: 17 |
Ok thanks for the clarification. The separation is ok, it is physical because of the low pressure, but seeing the results you really need a cavitation model because cavitation will happen. Actual results therefore are just "indicative " because they don't include cavitation. Btw are you getting convergence in this run? what is the order of your residuals?
|
|
July 6, 2014, 03:37 |
|
#19 | |
Member
Ben B. Huang
Join Date: Oct 2012
Posts: 54
Rep Power: 13 |
Quote:
it is converged after about 40 steps for the scenario with all three inlets opening(the exact scenario we just talk about before). see the fig plz. |
||
July 6, 2014, 03:55 |
|
#20 |
Senior Member
Blanco
Join Date: Mar 2009
Location: Torino, Italy
Posts: 193
Rep Power: 17 |
Ok for the convergence, btw it s really fast. Is the velocity you get at the outlet consistent with your experimental results?
|
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[blockMesh] non-orthogonal faces and incorrect orientation? | nennbs | OpenFOAM Meshing & Mesh Conversion | 7 | April 17, 2013 05:42 |
Negative Pressure in H2 gas flow and other physical interrogation | FloMol | ANSYS | 2 | April 9, 2012 19:57 |
[blockMesh] error message with modeling a cube with a hold at the center | hsingtzu | OpenFOAM Meshing & Mesh Conversion | 2 | March 14, 2012 09:56 |
negative pressure | mAx | FLUENT | 0 | January 25, 2006 14:31 |
a problem in calculating pressure drop in Fluent? | yu chun | FLUENT | 1 | May 18, 2004 03:40 |