CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > ANSYS Meshing & Geometry

[ICEM] Specifying Periodic Vertices Causes Mesh Overlap

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 22, 2010, 17:44
Default Specifying Periodic Vertices Causes Mesh Overlap
  #1
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 8
Josh is on a distinguished road
Hi all -

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



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:



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



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?
Josh is offline   Reply With Quote

Old   June 23, 2010, 14:53
Default Why Periodic?
  #2
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
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.
PSYMN is offline   Reply With Quote

Old   June 23, 2010, 15:12
Default
  #3
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 8
Josh is on a distinguished road
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 is offline   Reply With Quote

Old   June 24, 2010, 13:12
Default
  #4
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 8
Josh is on a distinguished road
I meant "free slip", not "freestream".
Josh is offline   Reply With Quote

Old   June 24, 2010, 14:03
Default Not sure.
  #5
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
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
PSYMN is offline   Reply With Quote

Old   June 24, 2010, 14:52
Default
  #6
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 8
Josh is on a distinguished road
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!
Josh is offline   Reply With Quote

Old   June 24, 2010, 18:24
Default
  #7
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
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
PSYMN is offline   Reply With Quote

Old   July 7, 2010, 15:53
Default
  #8
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 8
Josh is on a distinguished road
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 is offline   Reply With Quote

Old   July 7, 2010, 16:13
Default
  #9
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 8
Josh is on a distinguished road
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?
Josh is offline   Reply With Quote

Old   July 8, 2010, 00:19
Default Unstructured Mesh for Fluent
  #10
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
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... I am glad you figured it out on your own.
PSYMN is offline   Reply With Quote

Old   July 8, 2010, 02:39
Default
  #11
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 8
Josh is on a distinguished road
Thanks, as always, Simon. I should have realized that the first time through.
Josh is offline   Reply With Quote

Reply

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
[ICEM] Export unstructured periodic mesh from ICEM CFD to Fluent ivanddd ANSYS Meshing & Geometry 1 February 3, 2011 01:51
Meshing aifoil in ICEM student123a ANSYS Meshing & Geometry 13 December 8, 2010 11:40
TranformPoints gives skewed mesh Possible Bug andersking OpenFOAM Mesh Utilities 3 March 25, 2008 22:33
Convergence moving mesh lr103476 OpenFOAM Running, Solving & CFD 30 November 19, 2007 15:09
Icemcfd 11: Loss of mesh from surface mesh option? Joe CFX 2 March 26, 2007 18:10


All times are GMT -4. The time now is 16:50.