CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Mesh Generation & Pre-Processing Software > Pointwise & Gridgen

Axis Symmetric Mesh for OpenFOAM

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 25, 2020, 17:17
Post Axis Symmetric Mesh for OpenFOAM
  #1
Member
 
Gurpreet Singh
Join Date: Jan 2017
Posts: 36
Rep Power: 9
badwalgurpreet is on a distinguished road
Hi Pointwise Experts,

I am working on CFD simulation of axis symmetric problem using OpenFOAM as a solver and Pointwise a s a Meshing tool. I am attaching the geometry here for reference.

I am very new to Pointwise Meshing tool. I am looking for your valuable advice on this geometry to know whether Structured meshing is possible in this case or I should go for unstructured meshing.

(1)I want to make axis symmetric mesh for openfoam.

(2) I tried to make a simple axis symmetric mesh for cylinder using these steps..

* Made rectangle and created the connectors on it.
* Then I Created the dimensions on those four connectors.
* Created structured domain. Then I rotated the entire domain at an angle of 2.5 degrees using Edit - Transform- Rotate.

* I applied Extrude- Rotate command to rotate the entire domain at an angle of 5. degrees to make the Block.

* Applied all the boundary conditions like Wedge boundary conditions to front and back face.
* Exported the mesh using File- Export- CAE.



Can you please advise me how to mesh this type of complex geometry in Pointwise.

Regards
Gurpreet



1.jpg

Capture.jpg
badwalgurpreet is offline   Reply With Quote

Old   March 26, 2020, 09:44
Default
  #2
Member
 
Gurpreet Singh
Join Date: Jan 2017
Posts: 36
Rep Power: 9
badwalgurpreet is on a distinguished road
Can anyone help me ?
badwalgurpreet is offline   Reply With Quote

Old   March 26, 2020, 12:52
Post Pointwise Axisymmetric Mesh
  #3
Member
 
Gurpreet Singh
Join Date: Jan 2017
Posts: 36
Rep Power: 9
badwalgurpreet is on a distinguished road
Hi Dear,

I made Axis symmetric mesh of this geometry using Pointwise for OpenFOAM.
When I run the renumberMesh -overwrite utility, it runs without any problem. But the check mesh gives me one error like this *Wedge patch back not planar. Point (5.22212 1.74019 -0.0759782) is not in patch plane by 2.00397e-007 metre.
and I am attaching the picture here for reference. I also attaching the Pointwise Mesh file here.

You can find the fiels from the link below.

https://spaces.hightail.com/space/No2upnuVf7


Regards
Gurpreet
CheckMesh.PNG
badwalgurpreet is offline   Reply With Quote

Old   March 30, 2020, 12:56
Default
  #4
Senior Member
 
David Garlisch
Join Date: Jan 2013
Location: Fidelity Pointwise, Cadence Design Systems (Fort Worth, Texas Office)
Posts: 307
Rep Power: 14
dgarlisch is on a distinguished road
The errors reported by checkMesh are very small (~2e-7). These kinds of small deviations can be introduced by Pointwise because of numerical round-off errors during the generation of the domain points.

To fix, try this:
  • Create the un-extruded, symmetry domain.
  • Create a database plane entity in the same plane as the domain. Menu Create, Plane.
  • Project the domain's boundary AND interior points to this plane (this will constrain the domain and connectors to this plane). Menu Edit, Project.
  • Extrude-rotate this constrained domain.

Constraining the original domain and connectors to the plane will force all the points to be "highly planar" and should make OpenFOAM checkMesh happy.

To verify the domain constraints, select the domain and use Menu Examine, Database Associativity...
dgarlisch is offline   Reply With Quote

Old   April 25, 2020, 09:57
Default
  #5
New Member
 
Radhe
Join Date: Feb 2015
Posts: 11
Rep Power: 11
tanmay singhal is on a distinguished road
Quote:
Originally Posted by badwalgurpreet View Post
Hi Pointwise Experts,

I am working on CFD simulation of axis symmetric problem using OpenFOAM as a solver and Pointwise a s a Meshing tool. I am attaching the geometry here for reference.

I am very new to Pointwise Meshing tool. I am looking for your valuable advice on this geometry to know whether Structured meshing is possible in this case or I should go for unstructured meshing.

(1)I want to make axis symmetric mesh for openfoam.

(2) I tried to make a simple axis symmetric mesh for cylinder using these steps..

* Made rectangle and created the connectors on it.
* Then I Created the dimensions on those four connectors.
* Created structured domain. Then I rotated the entire domain at an angle of 2.5 degrees using Edit - Transform- Rotate.

* I applied Extrude- Rotate command to rotate the entire domain at an angle of 5. degrees to make the Block.

* Applied all the boundary conditions like Wedge boundary conditions to front and back face.
* Exported the mesh using File- Export- CAE.



Can you please advise me how to mesh this type of complex geometry in Pointwise.

Regards
Gurpreet



Attachment 75876

Attachment 75877
gurpreet,




did you use 2d or 3d option in Pointwise to generate the mesh for axisymmetric case?

Last edited by tanmay singhal; April 25, 2020 at 09:59. Reason: wrong syntax
tanmay singhal is offline   Reply With Quote

Old   April 26, 2020, 22:10
Default
  #6
Member
 
Gurpreet Singh
Join Date: Jan 2017
Posts: 36
Rep Power: 9
badwalgurpreet is on a distinguished road
Hi Dear,

I used 3d option .
badwalgurpreet is offline   Reply With Quote

Old   August 12, 2023, 11:09
Default
  #7
New Member
 
Deniz
Join Date: Mar 2023
Posts: 1
Rep Power: 0
Deniz58 is on a distinguished road
Quote:
Originally Posted by dgarlisch View Post
The errors reported by checkMesh are very small (~2e-7). These kinds of small deviations can be introduced by Pointwise because of numerical round-off errors during the generation of the domain points.

To fix, try this:
  • Create the un-extruded, symmetry domain.
  • Create a database plane entity in the same plane as the domain. Menu Create, Plane.
  • Project the domain's boundary AND interior points to this plane (this will constrain the domain and connectors to this plane). Menu Edit, Project.
  • Extrude-rotate this constrained domain.

Constraining the original domain and connectors to the plane will force all the points to be "highly planar" and should make OpenFOAM checkMesh happy.

To verify the domain constraints, select the domain and use Menu Examine, Database Associativity...
Hello Mr.Garlisch,

I did exactly what you said, but the error still persists. When I project onto the plane, the color of the errors turns purple. However, when I rotate, the color remains green after rotation. What could be the reason for this? I'm still getting the same error (*Wedge patch back not planar. exactly same as the above) using OpenFOAM.

Best regards

EDIT: I managed to solve the problem in a completely different way. Currently, openFOAM is not giving any errors. Still, thank you

Last edited by Deniz58; August 17, 2023 at 03:10.
Deniz58 is offline   Reply With Quote

Reply

Tags
axis symmetric, openfoam, pointwise

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[snappyHexMesh] problems generating clean mesh Christian_tt OpenFOAM Meshing & Mesh Conversion 2 June 20, 2019 05:39
Star CCM Overset Mesh Error (Rotating Turbine) thezack Siemens 7 October 12, 2016 11:14
3D Hybrid Mesh Errors DarrenC ANSYS Meshing & Geometry 11 August 5, 2013 06:42
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 11:55
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 19:49.