[Paraview] extract surface of multiblock mesh

[Chris Kees]

I turned off the overlapping domain decomposition (ghost cells) for a  
simple problem and the sequence

MergeBlocks->CleantoGrid->ExtractSurface->Clip

shows just the physical boundary of the problem (clipped open so you  
can see inside). Also volume visualization and streamline calculation  
works with no processor boundary artifacts.

 From what I understand, there are no filters in paraview or  
abstractions in the XDMF data model  at this time that will allow  
paraview to read in overlapping blocks and really make use of the  
ghost cells correctly. For now truncating our output to only "owned"  
elements will solve our problems. Thanks again for the help.

Chris

On Mar 30, 2009, at 2:06 PM, Chris Kees wrote:

> Thanks for  the help. I also tried suggestions from Paul, Ken, and  
> Berk, but it does seem that I'm stuck right now unless I provide  
> ParaView with more information. Since streamlines are computed  
> correctly on the current multiblock mesh I just generated the mesh  
> on a single processor and used ExtractSurface->Clip on that mesh to  
> visualize the geometry around the streamlines from the multiblock  
> grid.
>
> On the first method: Each of my UnstructuredGrids in the Multiblock  
> Grid is a subdomain in an overlapping decomposition of the domain.  
> Each of the subdomains has several elements of overlap (the layer of  
> ghost cells is more than one element thick).  Presumably the  
> streamline generation works now on the multiblock grid because the  
> overlap is loaded into ParaView. Is there a way I can just set a  
> cell-centered attributed to identify the ghost cells so that surface  
> extraction and volume visualization will work too?  Currently volume  
> visualization of the multiblock grid shows only a single subdomain  
> and volume visualization after MergeBlocks shows the whole domain  
> but with overlap regions being more opaque.
>
> On your other method, we have both the external boundary mesh and a  
> pre-mesh polygonal representation of the boundaries available in the  
> simulator. You are suggesting that I just dump one of those to a  
> valid ParaView format as well, is that correct?
>
> Chris
>
> On Mar 30, 2009, at 9:14 AM, Jean Favre wrote:
>
>> Chris Kees wrote:
>>> So far I've tried MergeBlocks->ExtractSurface->FeatureEdges->Clip  
>>> and
>>> various permutations that I've seen in previous posts and the wiki,
>>> but I always end up with the  surfaces on the interior of the tank  
>>> as
>>> if it still sees each subdomain as a closed surface.
>>
>> In fact, it seems to me that ParaView does the best it can. Your
>> unstructured mesh is partitioned in 512 pieces and [presumably],  
>> you did
>> not specify ghost-cells at the partition boundaries. Without
>> ghost-cells, ParaView has no information to help decide whether an
>> outside face looks towards the outside world, or to another  
>> partition. I
>> don't think any combination of filters would help you. Removing
>> duplicate points may only remove duplicate fake boundaries, but these
>> fake boundaries must be removed all together.
>>
>> I use two methods to achieve what you want. Ghost-cells, or another
>> multi-piece object containing the different boundary types (solid,
>> symmetries, inflow, outflow, etc) stored as vtkPolyData. These are  
>> read
>> in from the models on disk.
>>
>> Jean --
>> Swiss National Supercomputing Center
>>
>>
>>
>
> _______________________________________________
> Powered by www.kitware.com
>
> Visit other Kitware open-source projects at http://www.kitware.com/opensource/opensource.html
>
> Please keep messages on-topic and check the ParaView Wiki at: http://paraview.org/Wiki/ParaView
>
> Follow this link to subscribe/unsubscribe:
> http://www.paraview.org/mailman/listinfo/paraview