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

Flow over a flat plate as an immersed solid

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 21, 2012, 07:46
Default Flow over a flat plate as an immersed solid
  #1
Member
 
Hamed Abdul Majeed
Join Date: May 2012
Posts: 72
Rep Power: 5
hamed.majeed is on a distinguished road
Hi guys,
I used immersed solid approach in CFX for a flat plate to predict the boundary layer formation over it. I compared my results with a general case of flat plate, i.e. without using immersed solid domain. Although I know immersed solid under-predicts the boundary layer formation, however that is what I needed to find out.
This post is the gist of my analysis.
Earlier I have validated flow over a flat plate in cfx
Flat plate analysis in cfx

The flow parameters and references are same as defined in above link. I needed to change the geometry so that I could compare both the results.

Flow over a flat plate (general case)
Here is the model created.

Meshing

Then I applied the boundary conditions, the fluid domains need to be joined together by fluid fluid domain interface. Also wall b.c., inlet b.c. and symmetry b.c. are specified. At the exit i applied the outlet boundary condition.
This the the velocity contour I obtained.

Finally, I plotted the velocity vs Y plot, to see the boundary layer. The boundary layer thickness comes out to be 0.8 m. Which is quite good compared with the empirical value of 0.84m.


Flow over a flat plate as an immersed solid
I have done this part just to see how much the immersed solid approach under predicts the boundary layer.

# of iterations 100, variable variation 1e-4
I used ANSYS CFX v 14.0, so I used all the options related to Momentum source scaling factor and Boundary Model.
I used a range of Momentum source scaling factors and boundary models, these are the best results I could obtain.


The solution converged.
The velocity profile seems to be fairly accurate.



Finally, I calculated the velocity vs Y plot, which gives boundary layer thickness to be 0.105 m. The empirical value as stated earlier is 0.84 m.





Remarks
I have not done the mesh independency test yet, I shall soon post it.
The boundary layer is under predicted if immersed solid is used. This is clearly the case.




I plotted the friction coefficient vs length plot but they are very inaccurate, i problem I need to counter far.



Any comments and suggestions are appreciated.
hamed.majeed is offline   Reply With Quote

Old   July 21, 2012, 08:14
Default Momentum source scaling factor, Bondary Model
  #2
Member
 
Hamed Abdul Majeed
Join Date: May 2012
Posts: 72
Rep Power: 5
hamed.majeed is on a distinguished road
When a domain is defined as an immersed solid in ansys cfx, these two option are present that effect the analysis.

Momentum source scaling factor
It has a default value of 10. If we decrease it, accuracy will be affected.
Momentum source scaling factor decides the difference between the fluid velocity and the solid velocity at the immersed boundary.
As momentum source scaling factor is increased the fluid velocity is more closely equated to the solid velocity at the interface.
I have seen that a value of 50 or 100 is good enough.

Boundary Model > Boundary Tracking
In immersed solid forcing is applied to the fluid nodes that intersect with the solid nodes. Thus outside the immersed solid, the fluid has no forcing terms to account for the boundary layer. To better resolve the boundary effects CFX solver imposes a modified forcing term near the immersed boundary.
Thus boundary model specify the modified forcing.
To apply this modified forcing we need to first find the near wall node (Boundary tracking). Ansys uses two search algos for this purpose.
1.Search through elements
2. Boundary Face extrusion.
Search through elements need no input.
However Boundary face extrusion need the extrusion distance.
I found that the face extrusion distance should be greater than the 1st node distance from the wall (a property of the mesh, usually calculated of y+)


Also if proper extrusion distance is specified, boundary extrusion distance is more accurate than search through elements.

Please share anything further about these options. I also will.

They are very important in case of immersed solid approach in cfx.
hamed.majeed is offline   Reply With Quote

Old   July 22, 2012, 18:49
Default
  #3
Member
 
Felggv's Avatar
 
Felipe Gobbi
Join Date: Apr 2012
Location: Brazil
Posts: 76
Rep Power: 5
Felggv is on a distinguished road
Interesting comparison, it's always nice to see how different models work, the pros and cons may help others.
Felggv is offline   Reply With Quote

Old   May 28, 2013, 22:41
Default Sorry to bother you!I want to ask you a question about source momentun scaling factor
  #4
New Member
 
Join Date: Jul 2012
Posts: 25
Rep Power: 5
yuanmengyuan1989 is on a distinguished road
When I want to set source momentum scaling factor as 100, it will make error, and then I edit following command in the command editor.
FLOW: Flow Analysis 1
EXPERT PARAMETERS:
smooth inside ims = t
END
END

But it also make error as following:
ERROR #001100000 has occurred in subroutine EPORT_OBSOLETE_PRM. Message: The following unused Expert Solver Parameter was found: || SMOOTH INSIDE IMS | The parameter may be incorrectly spelled.
I do not know what leads to this error. And I see that you set the source momentum scaling factor as 200, so I want to know how it calculates smoothly.

Thnx! Wish you to reply to me!









Quote:
Originally Posted by hamed.majeed View Post
Hi guys,
I used immersed solid approach in CFX for a flat plate to predict the boundary layer formation over it. I compared my results with a general case of flat plate, i.e. without using immersed solid domain. Although I know immersed solid under-predicts the boundary layer formation, however that is what I needed to find out.
This post is the gist of my analysis.
Earlier I have validated flow over a flat plate in cfx
Flat plate analysis in cfx

The flow parameters and references are same as defined in above link. I needed to change the geometry so that I could compare both the results.

Flow over a flat plate (general case)
Here is the model created.

Meshing

Then I applied the boundary conditions, the fluid domains need to be joined together by fluid fluid domain interface. Also wall b.c., inlet b.c. and symmetry b.c. are specified. At the exit i applied the outlet boundary condition.
This the the velocity contour I obtained.

Finally, I plotted the velocity vs Y plot, to see the boundary layer. The boundary layer thickness comes out to be 0.8 m. Which is quite good compared with the empirical value of 0.84m.


Flow over a flat plate as an immersed solid
I have done this part just to see how much the immersed solid approach under predicts the boundary layer.

# of iterations 100, variable variation 1e-4
I used ANSYS CFX v 14.0, so I used all the options related to Momentum source scaling factor and Boundary Model.
I used a range of Momentum source scaling factors and boundary models, these are the best results I could obtain.


The solution converged.
The velocity profile seems to be fairly accurate.



Finally, I calculated the velocity vs Y plot, which gives boundary layer thickness to be 0.105 m. The empirical value as stated earlier is 0.84 m.





Remarks
I have not done the mesh independency test yet, I shall soon post it.
The boundary layer is under predicted if immersed solid is used. This is clearly the case.




I plotted the friction coefficient vs length plot but they are very inaccurate, i problem I need to counter far.



Any comments and suggestions are appreciated.
yuanmengyuan1989 is offline   Reply With Quote

Reply

Tags
flat plate, immersed boundary method, immersed solid

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
Flow Through an Immersed Solid ! kimiaghalam CFX 4 April 7, 2013 04:56
[ANSYS Meshing] Meshing for flat plate immersed solid hamed.majeed ANSYS Meshing & Geometry 0 July 10, 2012 13:32
Supersonic flow over a flat plate and a blunt body. Maddy FLUENT 0 August 31, 2010 16:35
compressible laminar flow over flat plate varunjain89 Main CFD Forum 17 March 25, 2010 00:51
Flow Over Flat Plate Lance FLUENT 1 November 13, 2008 23:20


All times are GMT -4. The time now is 02:31.