# A question in viscous and inviscid flow over an obstacle

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

 August 23, 2012, 07:32 A question in viscous and inviscid flow over an obstacle #1 Member   mhp Join Date: Dec 2011 Posts: 33 Rep Power: 6 Hi every body, As a general question does any separation occurs in the inviscid flows? I modeled a curved obstacle on a rigid wall in fluent for laminar flows but when I run the viscous and inviscid velocity contours it is obvious that there is a separation zones behind the obstacle in both cases, is there any problem? If it is not what is the explanation for it?

 August 23, 2012, 08:35 #2 Super Moderator   Oliver Gloth Join Date: Mar 2009 Location: Todtnau, Germany Posts: 116 Rep Power: 9 What is your boundary condition for the inviscid case? No-slip or slip wall?

August 23, 2012, 11:20
#3
Member

mhp
Join Date: Dec 2011
Posts: 33
Rep Power: 6
The boundary condition for wall and obstacle are no slip, and the mesh sketch is attached as a picture.
With attention to the fact that the velocity on the wall is zero,do you think that the separation point position is different from when a cylinder is in the flow (which in that case the B.C. should be changed to symmetry)?
Attached Images
 mesh structure 1.jpg (44.9 KB, 20 views)

 August 23, 2012, 11:27 #4 Senior Member   Join Date: Jul 2009 Posts: 232 Rep Power: 11 Why are you running an inviscid simulation with a no-slip boundary condition? If that is what you are doing, then that's your problem.

 August 23, 2012, 11:33 #5 Senior Member   Filippo Maria Denaro Join Date: Jul 2010 Posts: 2,593 Rep Power: 32 not at all, in inviscid flows the stream-lines follow the shape of the body... for example the classic theory of an inviscid flow around a cylinder, the total stagnation pressure is conserved, the static and the dynamic pressure along each stream-lines convert each other in a reversible way

 August 23, 2012, 11:40 #6 Member   mhp Join Date: Dec 2011 Posts: 33 Rep Power: 6 OK ,then so should I write UDF to define slip B.C. or there is more simple way to model an inviscid flow? The only thing that I do for inviscid flow is that in the Define/ model/ solver, I choose inviscid icon.

August 23, 2012, 11:43
#7
Senior Member

Filippo Maria Denaro
Join Date: Jul 2010
Posts: 2,593
Rep Power: 32
Quote:
 Originally Posted by agd Why are you running an inviscid simulation with a no-slip boundary condition? If that is what you are doing, then that's your problem.
I don't think that the no-slip BC can enter into the solution, in inviscid flow there is no molecular diffusion of momentum quantity that can transmit such condition ...

August 23, 2012, 11:58
#8
Senior Member

Join Date: Jul 2009
Posts: 232
Rep Power: 11
Quote:
 Originally Posted by FMDenaro I don't think that the no-slip BC can enter into the solution, in inviscid flow there is no molecular diffusion of momentum quantity that can transmit such condition ...
I'm aware of the physics. I was simply responding to the OP's statement that he is trying to model an inviscid flow using a no-slip BC. Doing that will create anomalous flow behavior, including spurious separation.

To the original poster - is there not a slip wall bc in the solver you are using? If not, then you will need to create one to properly model the flow as inviscid.

August 23, 2012, 12:05
#9
Senior Member

Filippo Maria Denaro
Join Date: Jul 2010
Posts: 2,593
Rep Power: 32
Quote:
 Originally Posted by agd I'm aware of the physics. I was simply responding to the OP's statement that he is trying to model an inviscid flow using a no-slip BC. Doing that will create anomalous flow behavior, including spurious separation. To the original poster - is there not a slip wall bc in the solver you are using? If not, then you will need to create one to properly model the flow as inviscid.

yes, but in a numerical code if you set no-slip conditions and have also zero molecular viscosity the solution is not influenced.. it remains only a graphical sketch to see the zero tangential velocity at wall, the solution should be correct ... otherwise in the code the viscosity is not set to zero and the no-slip bs is transmitted in the interior

August 23, 2012, 12:18
#10
Member

mhp
Join Date: Dec 2011
Posts: 33
Rep Power: 6
The problem begins when I want to compute the separation angle for the case which I sent the mesh condition picture in the above posts, from XY plot it was shown that this angle in different Re numbers is like the chart in the attached picture, but in the literature it is said that in the laminar flow a separation angle is about 80 deg. Is this because of the geometry and existence of the wall ?
Attached Images
 Separation angle.jpg (20.9 KB, 13 views) laminar separation 1.jpg (11.3 KB, 11 views)

 August 23, 2012, 12:22 #11 Senior Member   Filippo Maria Denaro Join Date: Jul 2010 Posts: 2,593 Rep Power: 32 I'm not sure to remember well, in 2D flow over a cylinder the laminar separation should be about 135 degree (maybe you can find it in the White book)... obviously in inviscid flow you must have no separation and a symmetric solution...

August 23, 2012, 12:44
#12
Member

mhp
Join Date: Dec 2011
Posts: 33
Rep Power: 6
Quote:
 Originally Posted by McEnroe I'm not sure to remember well, in 2D flow over a cylinder the laminar separation should be about 135 degree (maybe you can find it in the White book)... obviously in inviscid flow you must have no separation and a symmetric solution...
There is a table in Incropera book(7-7) that said in laminar flow the separation occurs in about 80 deg, but in turbulent flow because of high momentum, flow tends to attached to the boundary so that the separation point delay until about 140 deg, and my results show that the separation point in laminar flow over an obstacle and a wall with increase in Re number first stay in 135,then decrease and again about the end of regin for laminar flow increase to 135 deg. This is a big confusion for me and I can't explain the difference between this results and the simulations?

August 23, 2012, 13:47
#13
Senior Member

Join Date: Jul 2009
Posts: 232
Rep Power: 11
Quote:
 Originally Posted by FMDenaro yes, but in a numerical code if you set no-slip conditions and have also zero molecular viscosity the solution is not influenced.. it remains only a graphical sketch to see the zero tangential velocity at wall, the solution should be correct ... otherwise in the code the viscosity is not set to zero and the no-slip bs is transmitted in the interior
That is true as far as it goes; however, the significant velocity gradient will enter into any flux computations that involve the boundary nodes, i.e. face reconstruction of the velocity components. Those numerical effects will be transported into the flowfield in an unpredictable fashion. Additionally, any numerical viscosity will gradually diffuse the gradient into the interior of the domain.

August 24, 2012, 04:39
#14
Super Moderator

Oliver Gloth
Join Date: Mar 2009
Location: Todtnau, Germany
Posts: 116
Rep Power: 9
Hello,

Quote:
 yes, but in a numerical code if you set no-slip conditions and have also zero molecular viscosity the solution is not influenced..
This might not always be true.

1. Every code has some numerical dissipation and as a consequence your simulation could behave more like a viscous simulation with Re -> infinity. I don't think that anybody would argue that the flow reattaches if you crank up the free stream velocity more and more.

2. The values on the streamlines through the stagnation points are incorrect (zero velocity). Hence they will have some influence on the surrounding flow field.
Quote:
 not at all, in inviscid flows the stream-lines follow the shape of the body... for example the classic theory of an inviscid flow around a cylinder, the total stagnation pressure is conserved, the static and the dynamic pressure along each stream-lines convert each other in a reversible way
How could this be achieved if you force the dynamic pressure to be zero on a streamline.

Having said all that: It also depends on how the boundary condition is implemented. If it just influences the flux on the wall you might be right with the statement that it does not influence the solution. The momentum flux on the wall is a combination of pressure and shear stress. If the shear stress is zero than the pressure remains which is equivalent to a slip wall. If, however, the boundary condition puts a constraint on the actual values in the control-volume next to the wall, it will influence the solution. Maybe the Fluent theory manual could shed some light here.

Since the original poster reports a separated flow, I assume that there is some kind of influence. My advice would be to use a slip wall; maybe symmetry would work

Regards,
Oliver

EDIT: @agd: I missed your post in my reply -- What you say is pretty much what I was trying to explain. Unless there is a very specific flux condition for the wall the no-slip condition will influence the flow-field.

Last edited by ogloth; August 24, 2012 at 04:45. Reason: missed post by agd

 August 24, 2012, 05:01 #15 Senior Member   Filippo Maria Denaro Join Date: Jul 2010 Posts: 2,593 Rep Power: 32 the issue is quite complex since it involves the way in which the discretization near the wall is acted on ... I had experience in debugging a validating some codes, for example I can say that a FV code, I have written some time ago, based on flux BC, was tested on the lid-driven cavity for increasing Re number. Approaching Re -> infinity the solution is the rest because the shear of the lid cannot be trasmitted to the flow without molecular dissipation. In my code I used a third order upwidn scheme. I suppose that Fluent should implement the flux bc ...

 August 24, 2012, 05:13 #16 Super Moderator   Oliver Gloth Join Date: Mar 2009 Location: Todtnau, Germany Posts: 116 Rep Power: 9 One way to implement the BC is to have a mirrored ghost cell with the opposite velocity of the cell next to the wall. If you reconstruct the values on the face and compute the flux with those you might or might not get a tangential momentum transport. If I am not mistaken an upwind scheme would result in tangential momentum transport. As I said, the Fluent theory manual should be consulted.

 August 24, 2012, 07:50 #17 Senior Member   Filippo Maria Denaro Join Date: Jul 2010 Posts: 2,593 Rep Power: 32 This is just my opinion: - creating ghost nodes and calculating the values on them by extrapolation (that hence involves the prescribed value at wall) is typical for FD discretization. This is the way in which the solution can be affected by a wrong setting of the BC. - In FV you have to prescribe as BC the flux at the face that is adjacent to the wall. For inviscid flow you know exactly both diffusive and convective flux of the momentum equation, they are both zero. In no way the solution can be affected by the tangential velocity value. I am not an expert of Fluent but I suppose that being a FV code the setting of the BC should be on the fluxes.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post sylvain Main CFD Forum 5 August 2, 2013 16:48 Cath FLUENT 0 January 28, 2007 03:16 diaw Main CFD Forum 104 February 16, 2006 06:44 Axel Rohde Main CFD Forum 1 November 19, 2001 13:19 Adrin Gharakhani Main CFD Forum 13 June 21, 1999 05:18

All times are GMT -4. The time now is 00:41.