CFD Online URL
[Sponsors]
Home > Forums > OpenFOAM Native Meshers: blockMesh

Preview mesh in Paraview

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 12, 2009, 11:23
Default Hi I'm getting to grips with
  #1
New Member
 
Gareth
Join Date: Mar 2009
Posts: 24
Rep Power: 7
gareth__it_power is on a distinguished road
Hi
I'm getting to grips with the meshing in blockMeshDict, but find it frustrating that the only way to view the mesh is once I have applied all the initial conditions and run the model, then exporting to VTK and selecting wireframe. For some reason paraFoam does not work on my setup, so I can only use foamToVTK.

Is there a way to quickly export the mesh to paraView to have a look at it, after running blockMesh?

Many thanks

Gareth
gareth__it_power is offline   Reply With Quote

Old   March 25, 2009, 18:29
Default
  #2
New Member
 
James
Join Date: Mar 2009
Location: Sheffield, UK
Posts: 9
Rep Power: 7
derjames is on a distinguished road
you can use Salome (3.2.x) to draw the geometry and then create and visualise the mesh. When you finish, save the created mesh as IDEAS and then use the ideasToFoam tool to conver to OpenFOAM format. There is a tutorial about this at the caelinux website www.caelinux.com

hope this helps...

j
derjames is offline   Reply With Quote

Old   March 26, 2009, 09:26
Default
  #3
Member
 
Johannes Baumann
Join Date: Mar 2009
Location: Baden-Wuerttemberg, Germany
Posts: 42
Rep Power: 7
johannes is on a distinguished road
Hi Gareth,

another option would be to use the native OpenFOAM-Reader by Takuya Oshima.

It's the only ParaView post-processing method I'm using at the moment and I'm very satisfied with it. And - important for you - it's possible to visualize the mesh whether or not there are result files available for that case.

Best regards,

Johannes
johannes is offline   Reply With Quote

Old   March 16, 2011, 19:43
Default
  #4
sho
New Member
 
Son Ho
Join Date: Mar 2011
Location: Orlando, Florida
Posts: 5
Rep Power: 5
sho is on a distinguished road
Hello,

I am new at OF and starting to learn it with OpenFOAM 1.7.1 on Ubuntu 10.10 on VMWare Player. To develop a mesh using blockMesh, I follow the steps from the tutorial:

1. Edit blockMeshDict
2. Run blockMesh
3. Run paraFoam
4. View mesh on paraFoam
5. Quit paraFoam
6. Repeat step 1

My question is that how can I eliminate step 5 (and therefore step 3 in the following cycles) and get paraFoam to update and view the new mesh?

Thanks.
Son
sho is offline   Reply With Quote

Old   March 17, 2011, 03:49
Default
  #5
Senior Member
 
Martin
Join Date: Oct 2009
Location: Aachen, Germany
Posts: 252
Rep Power: 11
MartinB is on a distinguished road
Hi Son,

disable the "Cache Mesh" option (red arrow), click "Update GUI" option (green arrow) to enable the "Apply" button (just switch between On/Off all the time), click the "Apply" button (blue arrow). The updated mesh will be loaded and displayed.

Another feature, if you don't already use it, is to name the blocks in the blockMeshDict this way (be aware of "block_1" as a name for this block):

Code:
hex (15 9 52 58 23 16 59 66) block_1 (8 4 8) simpleGrading (1 1 1)
With the option "Include Sets" (yellow arrow) you can select the blocks to be shown in paraFoam. Disable the "internalMesh" option and select the blocks to be investigated instead.

Martin
Attached Images
File Type: png paraFoam.png (27.2 KB, 94 views)

Last edited by MartinB; March 17, 2011 at 03:50. Reason: Removed typos
MartinB is offline   Reply With Quote

Old   March 17, 2011, 12:59
Default
  #6
sho
New Member
 
Son Ho
Join Date: Mar 2011
Location: Orlando, Florida
Posts: 5
Rep Power: 5
sho is on a distinguished road
Thank you very much for the tips, Martin. I tried them out and it works perfectly.

I only have do the "disable Cache Mesh - enable Update GUI - click Apply" once. After that, I just have to click on the button "Refresh Times" in order to show the updated mesh (I use paraView 3.8.1 which came with openFoam 1.7.1 package).

Son
sho is offline   Reply With Quote

Old   June 3, 2011, 12:03
Default
  #7
New Member
 
Mike
Join Date: May 2011
Posts: 19
Rep Power: 5
mikemech is on a distinguished road
Hello,

Im trying to postprocess a mesh that I created with blockMesh, and I want to inspect separetely some blocks that I have saved in a "Sets" folder. I followed what MartinB said, but the problem is that Im using Paraview 3.10.1 on Windows XP. I cannot find the properties listed in Martin's screenshot in the object inspector!

Does anybody have an idea?
mikemech is offline   Reply With Quote

Old   June 3, 2011, 12:30
Default
  #8
Senior Member
 
Martin
Join Date: Oct 2009
Location: Aachen, Germany
Posts: 252
Rep Power: 11
MartinB is on a distinguished road
Hi Mike,

you can use foamToVTK this way:
Code:
foamToVTK -cellSet block_1
You will get additional .vtk files in the VTK folder and you can import the blocks independently.

Martin
MartinB is offline   Reply With Quote

Old   June 4, 2011, 13:13
Default
  #9
New Member
 
Mike
Join Date: May 2011
Posts: 19
Rep Power: 5
mikemech is on a distinguished road
Thanks Martin! It works perfectly
mikemech 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
Help with Mesh motion preview Mustafa Ayad FLUENT 2 January 20, 2009 23:40
mesh preview mode lee CD-adapco 2 June 16, 2007 06:10
Cannot preview the dynamic mesh sam FLUENT 4 May 26, 2005 07:58
Cannot preview mesh motion! dvinh FLUENT 0 August 18, 2004 00:44
about preview mesh motion lingo FLUENT 1 July 8, 2004 13:13


All times are GMT -4. The time now is 16:46.