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

Josh · July 20, 2011, 14:47

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.

ghorrocks · July 20, 2011, 19:33

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.

Josh · July 20, 2011, 23:12

Quote:

Originally Posted by ghorrocks

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

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.

ghorrocks · July 21, 2011, 08:09

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.

Josh · July 21, 2011, 16:47

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!

ghorrocks · July 21, 2011, 19:27

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.

Josh · July 22, 2011, 01:50

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.

July 20, 2011, 14:47	Warning error in Solver regarding mesh interpolation from 2D to 3D	#1
Josh Senior Member Joshua Counsil Join Date: Jul 2009 Location: Halifax, Nova Scotia, Canada Posts: 366 Rep Power: 17	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.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
[snappyHexMesh] snappyHexMesh won't work - zeros everywhere!	sc298	OpenFOAM Meshing & Mesh Conversion	2	March 27, 2011 21:11
Cells with t below lower limit	Purushothama	Siemens	2	May 31, 2010 21:58
OpenFOAM14 for Mac OSX Darwin 104	gschaider	OpenFOAM Installation	118	July 20, 2008 05:19
[blockMesh] Axisymmetrical mesh	Rasmus Gjesing (Gjesing)	OpenFOAM Meshing & Mesh Conversion	10	April 2, 2007 14:00
Mesh generator and CFD solver	Gennady Kireyko	Main CFD Forum	0	May 6, 2001 11:13

July 20, 2011, 19:33		#2
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,700 Rep Power: 143	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.

July 21, 2011, 08:09		#4
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,700 Rep Power: 143	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.

July 21, 2011, 16:47		#5
Josh Senior Member Joshua Counsil Join Date: Jul 2009 Location: Halifax, Nova Scotia, Canada Posts: 366 Rep Power: 17	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!

July 21, 2011, 19:27		#6
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,700 Rep Power: 143	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.

July 22, 2011, 01:50		#7
Josh Senior Member Joshua Counsil Join Date: Jul 2009 Location: Halifax, Nova Scotia, Canada Posts: 366 Rep Power: 17	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.