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

Warning error in Solver regarding mesh interpolation from 2D to 3D

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 20, 2011, 14:47
Default Warning error in Solver regarding mesh interpolation from 2D to 3D
  #1
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 9
Josh is on a distinguished road
Hey gang -

I have run many 2D simulations on various airfoils. I recently took my 2D grid and extended it 0.1c with 11 nodes in the spanwise direction to create a 3D grid. I was hoping to use a converged 2D solution as the initial condition for my 3D simulation. When I ran the simulation, Solver gave me the following warning:

The target mesh does not intersect with any source meshes that have the same domain type and motion. Skip the interpolation.


This seems to indicate that the 2D solution was not interpolated onto the 3D mesh. I found this confusing considering my 3D grid is identical to my 2D grid, but with differently named boundary conditions, differently named fluid, and a 0.1c span. I assumed CFX would just interpolate the 2D results across the 3D mesh as the initial condition, but this is not the case.

Is CFX incapable of interpolating a 2D solution to a 3D mesh? If it can do it, do you know what I've done wrong?

Thanks for any help.
Josh is offline   Reply With Quote

Old   July 20, 2011, 19:33
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,959
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
The domain for your 3D model is longer than the 2D, isn't it? In that case the interpolator probably won't match it up properly.

Alternately it could be a bug in the interpolator. If you suspect this I would talk to CFX support about it.
ghorrocks is offline   Reply With Quote

Old   July 20, 2011, 23:12
Default
  #3
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 9
Josh is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
The domain for your 3D model is longer than the 2D, isn't it? In that case the interpolator probably won't match it up properly.
Surprisingly, no. I exported the 2D mesh as a 2D Fluent mesh and CFX Pre automatically extruded it as 0.4 m long in the negative z direction (one element deep). The 3D mesh is 0.1 m thick in the positive z direction with 10 elements.

Quote:
Originally Posted by ghorrocks View Post
Alternately it could be a bug in the interpolator. If you suspect this I would talk to CFX support about it.
I sent them a report. They told me to try running it with "Continue History From..." unchecked in the run definition. This is supposed to eliminate some of the mesh checks. The same error occurred.

Thanks, as always, Dr. H.
Josh is offline   Reply With Quote

Old   July 21, 2011, 08:09
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,959
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
I think that is your problem. The interpolator is pretty dumb - if the meshes do not overlap in space it does not match them. So if your 2D mesh is in -z and the 3D mesh is in +z then you get no overlap and the interpolator does not map anything across.

I would translate the 3D mesh so it sits inside the 2D mesh in 3D space (if you know what I mean ) and the interpolator should work fine. A translation of 0.3m in the -z direction should do it.
ghorrocks is offline   Reply With Quote

Old   July 21, 2011, 16:47
Default
  #5
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 9
Josh is on a distinguished road
That's what I was afraid of. Unfortunately, the 0.1 m extrusion is done purposefully as this specific case has been shown to be span-independent from about 0.1c to 0.3c, though the thinner it is, the better - 0.1c span with 10 nodes is better resolved than 0.3c with 10 nodes. Still, it might be worth trying.

Thanks!
Josh is offline   Reply With Quote

Old   July 21, 2011, 19:27
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,959
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
No, I am not proposing changing your extrusion length, just the position in space where it sits. You will still have a 0.1m extrusion length. So instead of the mesh lying from z=0 to z=0.1, translate it to z=-0.3 to z=-0.2. Still a 0.1m extrusion, but translated a bit in z.
ghorrocks is offline   Reply With Quote

Old   July 22, 2011, 01:50
Default
  #7
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 9
Josh is on a distinguished road
Not only did your suggestion work, you beat the ANSYS support team to the answer, and I told them about it before posting here.

Thanks again, Dr. Glenn.
Josh is offline   Reply With Quote

Reply

Tags
interpolation, mesh, solver, three-dimensional, two-dimensional

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
snappyHexMesh won't work - zeros everywhere! sc298 OpenFOAM Native Meshers: snappyHexMesh and Others 2 March 27, 2011 21:11
Cells with t below lower limit Purushothama CD-adapco 2 May 31, 2010 21:58
OpenFOAM14 for Mac OSX Darwin 104 gschaider OpenFOAM Installation 118 July 20, 2008 05:19
Axisymmetrical mesh Rasmus Gjesing (Gjesing) OpenFOAM Native Meshers: blockMesh 10 April 2, 2007 14:00
Mesh generator and CFD solver Gennady Kireyko Main CFD Forum 0 May 6, 2001 11:13


All times are GMT -4. The time now is 04:24.