CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (http://www.cfd-online.com/Forums/ansys-meshing/)
-   -   [ICEM] Specifying Periodic Vertices Causes Mesh Overlap (http://www.cfd-online.com/Forums/ansys-meshing/77430-specifying-periodic-vertices-causes-mesh-overlap.html)

Josh June 22, 2010 17:44

Specifying Periodic Vertices Causes Mesh Overlap
 
Hi all -

I'm having some trouble specifying periodicity for a structured H-grid around an airfoil, shown below.

http://img22.imageshack.us/img22/272/periodicity1.jpg

I want to create a periodic boundary condition on the yellow lines shown above. I am exporting to ANSYS CFX (Pre). I already defined periodicity in the Global Mesh Setup. Now, I'm trying to specify that the vertices within the two red circles are periodic with each other, and the vertices within the two purple circles are periodic with each other. I use Blocking > Edit Block > Periodic Vertices > Create, then choose the desired vertices. When I try making the vertices within the red circles periodic, the following overlap occurs:

http://img651.imageshack.us/img651/2...riodicity2.jpg

Similarly, for with the same procedure for the purple circle vertices:

http://img411.imageshack.us/img411/9...riodicity3.jpg

I've associated my vertices to points at those locations, so I don't know why this is occurring. Can anyone help?

Also, is it even necessary to set these vertices as periodic when exporting to CFX? That is, can I get away with just setting the global periodicity in the Global Mesh Setup, then worry about specifying which boundaries are periodic in CFX Pre?

PSYMN June 23, 2010 14:53

Why Periodic?
 
Did you setup a translational periodicity in Y with the correct Delta Y? Double check that. This should work perfectly fine, so I am guessing user error, but you can send me your file and I will check it for you.

In answer to your question, no, setting the global periodicity settings is not enough to ensure periodic Hexa. You must make the blocking periodic so that the mesh will be periodic or CFX/Fluent (or any other solver as far as I know) will give you an error when you try to apply a periodic boco.

However, this sort of far field doesn't typically even need periodicity... Why are you trying to apply it? Certainly applying it to a section of the far field (when the far field geometry its self is not periodic) is very unusual.

Josh June 23, 2010 15:12

Thanks, as always, Simon.

Would you suggest using a freestream BC? I've been doing internal aerodynamics recently and was just creating the periodicity out of habit, I suppose.

Josh June 24, 2010 13:12

I meant "free slip", not "freestream".

PSYMN June 24, 2010 14:03

Not sure.
 
Not sure... I have done this before and used a velocity inlet along the entire "C". On those sides, the vector is along the wall, so it acts like free slip (it worked for me anyway).

However, I usually use a Tunnel (with regular inlet and outlet and frictionless walls), so I am not sure what the best approach for this shaped far field would be.

Perhaps ask that question on the Fluent Forum.

Simon

Josh June 24, 2010 14:52

Thanks, Simon. I was considering that, as well.

One more problem, if you don't mind. This is the first time I've had this happen. I created my 2D planar blocking scheme, meshed it, created the parts based on curves (e.g., inlet, outlet...), and am happy with the quality, aspect ratio, etc. I converted the pre-mesh to an unstructured mesh, then extruded it as one element deep. Normally, with the inherited part names option on, the boundary condition curves become 3D curves/surfaces, at which point I import the file into CFX. However, this time, the parts remained as 2D curves, so CFX does not recognize any of the boundary conditions (that is, there is a "3D" extruded mesh, but the part names still only apply to the original curves). I tried creating new parts using entities (selecting each individual grid element), which worked fine for the inlet and outlet BCs, but this is extremely difficult to pull of for the airfoil and symmetry boundaries. Is there something I'm doing wrong? Is there an easier way to create BCs that CFX will recognize?

Thanks!

PSYMN June 24, 2010 18:24

Extrude with inherited should have done it (line element parts become shells)... Not sure why it wouldn't.

But if you are using a recent version of CFX, you could just keep it 2D and export a Fluent mesh. Apparently, CFX is smart enough to recognize a 2D Fluent Mesh and automatically extrude it for you during import.

Let me know how that works for you as I haven't got around to trying it for myself.

Simon

Josh July 7, 2010 15:53

Simon -

Sorry for taking so long to respond. We were updating our license server.

I am using a newer version of CFX (12.1), so I tried your suggestion. I saved the ICEM file as a 2D Fluent mesh. I then imported the .msh file into CFX-Pre using the Import Mesh > FLUENT option. The 2D mesh was automatically extruded. However, not all of the parts were recognized.

As a starting point, I always like to follow your YouTube tutorial (http://www.youtube.com/watch?v=EknKV...eature=related). However, additionally to the farfield and curves boundary conditions, I like to create a new BC for the outlet. Although CFX recognized the farfield and curves boundary conditions I created in the same style you did, it didn't recognize the outlet condition. Instead, when imported into Pre, the outlet is still part of the farfield BC.

Josh July 7, 2010 16:13

Fixed.

The problem was that I created my outlet boundary condition AFTER I created my mesh. I went back, updated my pre-mesh, converted the mesh to unstructured, then outputted it.

On that note, with a Fluent mesh, is it necessary to convert the pre-mesh to unstructured, or is it wiser to convert it to a multi-block mesh?

PSYMN July 8, 2010 00:19

Unstructured Mesh for Fluent
 
Fluent is an unstructured solver, so unstructured mesh is what it wants ;)


And yes, the 2D boundary bocos are applied to line elements (not curves)... In order to have line elements in the outlet part, you must associate and edge with a curve in the outlet part first and then generate the premesh and convert that to an unstructured mesh... It really sounds more complicated than it is when I type it out that way...:o I am glad you figured it out on your own.

Josh July 8, 2010 02:39

Thanks, as always, Simon. I should have realized that the first time through.


All times are GMT -4. The time now is 20:59.