Flow over a flat plate as an immersed solid
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
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.
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.
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.
Momentum source scaling factor, Bondary Model
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.
Interesting comparison, it's always nice to see how different models work, the pros and cons may help others.
Sorry to bother you！I want to ask you a question about source momentun scaling factor
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
smooth inside ims = t
But it also make error as following:
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.
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.
Thnx! Wish you to reply to me!
|All times are GMT -4. The time now is 06:49.|