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

Autogrid export CGNS mesh only with multiple base nodes???

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

Like Tree1Likes
  • 1 Post By DarylMusashi

Reply
 
LinkBack Thread Tools Display Modes
Old   January 21, 2017, 14:21
Default Autogrid export CGNS mesh only with multiple base nodes???
  #1
swm
Member
 
swm's Avatar
 
Join Date: Dec 2013
Posts: 47
Rep Power: 6
swm is on a distinguished road
Hi guys,

I've encountered a strange problem which keeps puzzling me for a week
I exported a mesh with CGNS format in Numeca Autogrid and then imported it with Pointwise, but it failed!

The error message is clear: 'File contains multiple base nodes'. I also looked it up in the User manual which told me pointwise could only load CGNS mesh with single base node.

I'm wondering when I export CGNS mesh in Autogrid, whether I set something correct or just need to modify some parameters to make pointwise can load the kind of CGNS mesh.

Does anybody have any suggestion or solution? (Although I can export the mesh in Autogrid with Plot3D format, it loses all the BC info which is critical to show the connection between multiple blocks. So that I have to export it with CGNS format)

Many thanks.
swm is offline   Reply With Quote

Old   January 21, 2017, 17:07
Default
  #2
Senior Member
 
DarylMusashi's Avatar
 
Holger Dietrich
Join Date: Apr 2011
Location: Germany
Posts: 136
Rep Power: 8
DarylMusashi is on a distinguished road
Dear swm,

indeed AutoGrid5 CGNS files contain several bases. I found the following passages in the IGG manual:

"A CGNS base contains the information on the mesh blocks, their connectivity and boundary conditions. IGG™/AutoGrid5™ can write several bases, they are described hereafter according to their name. The first one is mandatory for a computation, the other ones are optional and not always present.

Base#1
This base is the main one and contains the useful information about the mesh to be run by the solver.

Butterfly_base
This base contains mesh information for the parent block of a butterfly topology. Internal use only.

meridional_base
For a turbomachinery mesh, contains a meridional mesh that will be used by FINE™/Turbo for the computation initial solution. Internal use only.

tools_base
This base contains information for post processing and some other information for AutoGrid. Internal use only."


You could give it a try and manipulate the AutoGrid5 CGNS file with ADFViewer. Its part of CGNSTools, which can be downloaded here, for example: https://sourceforge.net/projects/cgns/files/cgnstools/, Release 2 contains a windows version.

After installation you can read in CGNS files. In the attached screenshot you can see the different bases from a typical AutoGrid5 file. With right-clicking you can delete the meridional and tools base, for example. The turbulent data bases in my example only exist if FINE/Turbo did calculations on this mesh, so they shouldn't be there in your case.

After deleting all unnecessary bases except "Base#1" maybe Pointwise is able to read the mesh now. May I ask why and how you want to further modify the mesh in Pointwise?
Attached Images
File Type: jpg aachen_ADF.JPG (71.9 KB, 19 views)
swm likes this.

Last edited by DarylMusashi; January 22, 2017 at 03:16.
DarylMusashi is offline   Reply With Quote

Old   January 21, 2017, 21:28
Default
  #3
swm
Member
 
swm's Avatar
 
Join Date: Dec 2013
Posts: 47
Rep Power: 6
swm is on a distinguished road
Hi Holger,

Thank you for your suggestion. The software you recommend is downloaded easily but the SETUP.exe can not work in my laptop (WINDOWS10).

Actually I won't use Eurans to run CFD cases but just use Autogrid to generate grid as fast as possible. A set of in-house CFD code developed by ourselves will be used to solve CFD problems. But it can only accept plot 3D grid and BC conditions written in Gridgen Generic format. So that I have to convert the format by Gridgen or Pointwise.

This finite volume solver can only handle structured multiblocks. If I want to increase the computational efficiency with MPI, I have to split some blocks to make each core have equal nodes approximately. Moreover, the mesh generated by Autogrid automatically can not meet the requirement of DES/LES computation in some cases, you'd better improve the mesh quality in some critical region by more powerful mesh generator, such as Pointwise.

Thanks for your help.

swm
swm is offline   Reply With Quote

Old   January 21, 2017, 21:30
Default
  #4
swm
Member
 
swm's Avatar
 
Join Date: Dec 2013
Posts: 47
Rep Power: 6
swm is on a distinguished road
Hi Holger,

Thank you for your suggestion. The software you recommend is downloaded easily but the SETUP.exe can not work in my laptop (WINDOWS10).

Actually I won't use Eurans to run CFD cases but just use Autogrid to generate grid as fast as possible. A set of in-house CFD code developed by ourselves will be used to solve CFD problems. But it can only accept plot 3D grid and BC conditions written in Gridgen Generic format. So that I have to convert the format by Gridgen or Pointwise.

This finite volume solver can only handle structured multiblocks. If I want to increase the computational efficiency with MPI, I have to split some blocks to make each core have equal nodes approximately. Moreover, the mesh generated by Autogrid automatically can not meet the requirement of DES/LES computation in some cases, you'd better improve the mesh quality in some critical region by more powerful mesh generator, such as Pointwise.

Thanks for your help.

swm
swm is offline   Reply With Quote

Old   January 21, 2017, 21:32
Default
  #5
swm
Member
 
swm's Avatar
 
Join Date: Dec 2013
Posts: 47
Rep Power: 6
swm is on a distinguished road
Hi Holger,

Thank you for your suggestion. The software you recommend is downloaded easily but the SETUP.exe can not work in my laptop (WINDOWS10).

Actually I won't use Eurans to run CFD cases but just use Autogrid to generate grid as fast as possible. A set of in-house CFD code developed by ourselves will be used to solve CFD problems. But it can only accept plot 3D grid and BC conditions written in Gridgen Generic format. So that I have to convert the format by Gridgen or Pointwise.

This finite volume solver can only handle structured multiblocks. If I want to increase the computational efficiency with MPI, I have to split some blocks to make each core have equal nodes approximately. Moreover, the mesh generated by Autogrid automatically can not meet the requirement of DES/LES computation in some cases, you'd better improve the mesh quality in some critical region by more powerful mesh generator, such as Pointwise.

Thanks you for your help.

swm
swm is offline   Reply With Quote

Old   January 22, 2017, 03:09
Default
  #6
Senior Member
 
DarylMusashi's Avatar
 
Holger Dietrich
Join Date: Apr 2011
Location: Germany
Posts: 136
Rep Power: 8
DarylMusashi is on a distinguished road
Dear swm,

thank you for your detailed answer. To be more precise I downloaded the installation package "win 2-5-2" yesterday: https://sourceforge.net/projects/cgn...20Release%202/. This worked properly for me and I use Windows 10, too. Maybe you want to check your security settings or share the error during installation?

Secondly, I understand your problem with splitting the blocks equally for MPI parallel computations. You could do this easily in IGG with the "split block" function in the top left control bar after you have generated your mesh in AutoGrid.

May I ask which mesh regions or quality criteria are not satisfying for you? You say Pointwise is more powerful than AutoGrid. Does it have additional features for mesh creation or is it only more user friendly and gives you more control over the parameters? I strongly suppose the latter.

Finally, maybe its interesting for you to know, that FINE/Turbo is capable of DES computations. ("The DES (Detached Eddy Simulations) model has been implemented in FINE™/Turbo. For more information, please contact your local support office."). Secondly, FINE/Turbo solver is able to use a "parallel partioned" technique, so it splits the blocks automatically for perfect load balancing.

Kind regards
Holger
DarylMusashi 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
3D Hybrid Mesh Errors DarrenC ANSYS Meshing & Geometry 11 August 5, 2013 06:42
2D Mesh Generation Tutorial for GMSH aeroslacker Open Source Meshers: Gmsh, Netgen, CGNS, ... 12 January 19, 2012 04:52
OpenFOAM on MinGW crosscompiler hosted on Linux allenzhao OpenFOAM Installation 127 January 30, 2009 20:08
How to control Minximum mesh space? hung FLUENT 7 April 18, 2005 09:38
CFX4.3 -build analysis form Chie Min CFX 5 July 12, 2001 23:19


All times are GMT -4. The time now is 13:56.