[raye_xie]

Hello,

I was trying to mesh an airfoil with Pointwise to run in OpenFOAM (mesh shown in attached pictures). When I export CAE with 2D option, I have error says "The grid is not Z-planar". When I extruded all the domains by 1, and export CAE with 3D options, I got one mesh check failed in openFOAM says "Number of edges not aligned with or perpendicular to non-empty directions: 16134". When I zoom in to look at my mesh (from Y direction), it seems that all my unstructured domains are not perfectly on the same plane (They are all supposed to be on Z plane).

I would really appreciate it if anyone could give me some advice!

-Raye

[dgarlisch]

Using your original 2D grid:

1. Create an appropriate Z plane (=0?)
   • Create, Planes...
2. Project all domains onto the plane
   • Select all domains
   • Edit, Project...
   • Linear projection
   • Use Z-Axis
   • Uncheck Interior Only
   • Project
   • OK
3. Orient all domain normals to +Z
   • Select all unstructured domains
   • Edit, Orient...
   • ...stuff...
   • OK
   • Select all structured domains
   • Edit, Orient...
   • ...stuff...
   • OK
4. Export grid
   • Select all domains
   • File, Export, CAE...

[raye_xie]

Thank you so much, David! This is super helpful!

Originally Posted by dgarlisch

Using your original 2D grid:

1. Create an appropriate Z plane (=0?)
   • Create, Planes...
2. Project all domains onto the plane
   • Select all domains
   • Edit, Project...
   • Linear projection
   • Use Z-Axis
   • Uncheck Interior Only
   • Project
   • OK
3. Orient all domain normals to +Z
   • Select all unstructured domains
   • Edit, Orient...
   • ...stuff...
   • OK
   • Select all structured domains
   • Edit, Orient...
   • ...stuff...
   • OK
4. Export grid
   • Select all domains
   • File, Export, CAE...

[RcktMan77]

This approach might be a little quicker and more straightforward:

https://www.youtube.com/watch?v=A2Wp...ature=youtu.be

[adi.ptb]

Hi all,

I've got a similar problem with my mesh. I have a structured mesh that I can export to OpenFOAM without an issue. However, when I run the simulation the solver cuts out. I'm pretty much sure that the problem is with the mesh since I've completed the simulation using a hybrid mesh that was created in another mesh generator.

This is how I figured out that the problem is with the mesh:
Instead of setting the dimension to 3D I chose 2D as the dimension and allowed the Pointwise to create the front and back faces for OpenFOAM. When I tried to export the 2D mesh Poinwise prompted that "The grid is not Z-planar" and thats how I ended up here.

It seems that non of the solutions posted here work for me. I followed David's approach and when I projected all the domains into the Z plane I ended up with a distorted shape, not to mention that 10% of the points were still off.

Then I used Zack's approach and scaled the domains and then oriented all the domains based on the right hand rule. At this point I was able to export the 2D mesh. But, the solver still cuts out. Here is the link to the mesh in case someone wants to look at it. I would appreciate any help.


https://www.dropbox.com/s/9z6t02iuw4...ceMesh.pw?dl=0

[dgarlisch]

There are several problem here:

• All the domains are in the Z=4242.6401 plane
• The grid extents (far field) are way too big compared to the airfoil chord length (330K vs. 1.2K).
• The initial BL spacing (0.00013) vs. the grid extents (330K) is ~9 orders of magnitude.

All this combined exceeds machine precision and will most likely result in unstable calculations during export.

Suggestions to maximize numerical precision:

• Move 2D domains to Z=0.0
• Make farfield/chord ratios more reasonable.

CORRECTION:
The CFD guys around here say to capture flow details:

• 10x body length upstream and downstream should suffice for an entire aircraft.
• 100x chord length upstream and downstream should suffice for a standalone airfoil.

Good luck.

[adi.ptb]

David,

Thanks for your response. I've modified the grid based on your suggestions. The problem is not solved though. Here is the link to the modified mesh. Any further suggestions?



https://www.dropbox.com/s/mr6rkq8y82...jected.pw?dl=0

[dgarlisch]

As best I can tell, the grid exported from Pointwise is topologically correct. However, it still has mesh quality issues.

You have exceeded my ability to help. Others will need to chime in.

Also, you can contact Pointwise support for more help. Please refer them to this post for background.


FYI, I did run the OpenFOAM checkMesh utility on the exported grid and got this:

> checkMesh -case scratch
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.3.1 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.3.1-bcfaaa7b8660
Exec : checkMesh -case scratch
Date : Feb 05 2018
Time : 12:22:14
Host : "xxxx"
PID : 21119
Case : ./scratch
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create polyMesh for time = 0

Time = 0

Mesh stats
points: 386872
internal points: 0
faces: 771370
internal faces: 384494
cells: 192644
faces per cell: 6
boundary patches: 5
point zones: 0
face zones: 0
cell zones: 0

Overall number of cells of each type:
hexahedra: 192644
prisms: 0
wedges: 0
pyramids: 0
tet wedges: 0
tetrahedra: 0
polyhedra: 0

Checking topology...
Boundary definition OK.
Cell to face addressing OK.
Point usage OK.
Upper triangular ordering OK.
Face vertices OK.
Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces...
Patch Faces Points Surface topology
farfield 958 1916 ok (non-closed singly connected)
wall_airfoil 307 614 ok (non-closed singly connected)
wall_flap 165 330 ok (non-closed singly connected)
wall_slat 158 316 ok (non-closed singly connected)
BaseAndTop 385288 386872 ok (non-closed singly connected)

Checking geometry...
Overall domain bounding box (-6600 -7006.06 0) (7473.95 7067.82 20.1838)
Mesh (non-empty, non-wedge) directions (1 1 0)
Mesh (non-empty) directions (1 1 0)
All edges aligned with or perpendicular to non-empty directions.
Boundary openness (1.01392e-19 -2.94824e-20 -2.66931e-15) OK.
***High aspect ratio cells found, Max aspect ratio: 90600.7, number of cells 219
<<Writing 219 cells with high aspect ratio to set highAspectRatioCells
Minimum face area = 9.9805e-05. Maximum face area = 106309. Face area magnitudes OK.
Min volume = 0.00201444. Max volume = 2.14571e+06. Total volume = 3.13831e+09. Cell volumes OK.
Mesh non-orthogonality Max: 89.749 average: 13.984
*Number of severely non-orthogonal (> 70 degrees) faces: 585.
Non-orthogonality check OK.
<<Writing 585 non-orthogonal faces to set nonOrthoFaces
Face pyramids OK.
Max skewness = 1.2188 OK.
Coupled point location match (average 0) OK.

Failed 1 mesh checks.

End

[dgarlisch]

Please see correction above.

Also, be sure to run renumberMesh on the exported grid BEFORE running solver.

[adi.ptb]

Hi David,

I have revised the mesh based on your recommendations and I can see that the quality of the mesh has increased. I created a plane at z =0 and projected all the domains to that plane. Then I oriented all the domains based on the right hand rule. Then I did the simulation with CFX without any issues. However, OpenFOAM still complains about the mesh and I can't pass all the mesh checks and when I run the simulation the solution diverges in the first few iterations. I did renumberMesh -overwrite before running the simulation. You can access the mesh file and the OpenFOAM case setup from the link below. Any other recommendations before I give up on OpenFOAM?


https://www.dropbox.com/s/cx0fvv13co...Setup.zip?dl=0

[dgarlisch]

I am not OF experienced. Others will need to chime in here.

One thing I did notice is the 2D thickness of your grid was 0.5 exactly. It looks like you exported to OF using the already thickened grid in 30P-30N_VolumeMesh_RRR_Projected.pw.

Have you tried exporting to OF using the 2D grid? When exporting from 2D, the grid is automatically thickened to one cell during export.

In CAE, Set Solver Attributes... you can change the thickness. The default of 0.0 will automatically chose a thickness that is the average edge length of the 2D grid. This default was suggested to us by the very experienced OF users at Applied CCM.

Try running the grid exported from 2D using the default thickness.

You will need to set your BCs and VCs in 2D mode before exporting.

Good luck.

[adi.ptb]

David,

Thanks for your response. I did that. It didn't have any effects.

[dgarlisch]

Originally Posted by adi.ptb

David,

Thanks for your response. I did that. It didn't have any effects.

I have reached the limit of my knowledge. Others will need to chime in.

It might help to post the output from checkMesh and any other relevant warning/error messages from OF.

[adi.ptb]

Create time

Create polyMesh for time = 0

Time = 0

Mesh stats
points: 536678
internal points: 0
faces: 1069677
internal faces: 532995
cells: 267112
faces per cell: 6
boundary patches: 6
point zones: 0
face zones: 0
cell zones: 0

Overall number of cells of each type:
hexahedra: 267112
prisms: 0
wedges: 0
pyramids: 0
tet wedges: 0
tetrahedra: 0
polyhedra: 0

Checking topology...
Boundary definition OK.
Cell to face addressing OK.
Point usage OK.
Upper triangular ordering OK.
Face vertices OK.
Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces...
Patch Faces Points Surface topology
frontAndBackPlanes 534224 536678 ok (non-closed singly connected)
inlet 1014 2030 ok (non-closed singly connected)
outlet 565 1132 ok (non-closed singly connected)
wall_airfoil 440 880 ok (non-closed singly connected)
wall_flap 220 440 ok (non-closed singly connected)
wall_slat 219 438 ok (non-closed singly connected)

Checking geometry...
Overall domain bounding box (-124.73451 -125 0) (125 125 0.5)
Mesh has 2 geometric (non-empty/wedge) directions (1 1 0)
Mesh has 2 solution (non-empty) directions (1 1 0)
All edges aligned with or perpendicular to non-empty directions.
Boundary openness (-2.222464e-019 -1.1775465e-021 4.5947381e-018) OK.
***High aspect ratio cells found, Max aspect ratio: 20774.904, number of cells 34759
<<Writing 34759 cells with high aspect ratio to set highAspectRatioCells
Minimum face area = 3.0045e-008. Maximum face area = 42.130928. Face area magnitudes OK.
Min volume = 1.50225e-008. Max volume = 21.065464. Total volume = 27878.276. Cell volumes OK.
Mesh non-orthogonality Max: 87.732302 average: 13.86317
*Number of severely non-orthogonal (> 70 degrees) faces: 380.
Non-orthogonality check OK.
<<Writing 380 non-orthogonal faces to set nonOrthoFaces
Face pyramids OK.
Max skewness = 1.061713 OK.
Coupled point location match (average 0) OK.

Failed 1 mesh checks.

End