[Paraview] Exporting ICEM CFD Mesh to ParaView

Thu Jan 21 07:16:31 EST 2010

Hi,

thank you all for the attention. I've found a way to force ICEM CFD to
export the parts.

I used to export to Exodus II format by clicking on File -> Export Mesh ->
To Exodus -> Write Exodus Input File. This exports only the mesh and element
blocks. To export also the 2D parts, one can create "dummy" boundary
conditions on them, by going to File -> Export Mesh -> To Exodus -> Exodus
Family Attributes, selecting the part, clicking on "Create New" and "Side
Set" type of Boundary Condition. Then you can write the exodus input like
before. One has to do it for each part he wants to export, so, this can be
really annoying for large number of components. But this solves my problem
for now !

Thanks again,
Rafael Castañeda.

2010/1/19 Samuel Key <samuelkey at bresnan.net>

>  Rafael,
>
> *Exodus II.*  The Exodus-II format supports side-sets and node-sets, each
> of which may have point-data and cell-data.  These are subsets of the mesh
> model (meshed domain, whole object, or whatever terminology you are using).
> On input, they are intended to be used by the simulation software for areal
> and point BCs.  If the simulation wants to place data on these side-sets and
> node-sets, it may and then the results can be viewed with ParaView.  The
> side-sets in the case of solids are element faces, and in the case of planar
> elements (quads or triangles in 3D) are element edges. If one wants to use
> one of these auxiliary sets for the display of results, a side-set can
> transect any number of element blocks, have no BC's "attached" to it, but
> have the simulation code add data to it.  Of course, the simulation code has
> to recognize this and write the datum occurring of this side-set out to the
> final results.
>
> An Exodus-II file used only for mesh & BC input and empty of results is
> usually referred to as a "Genesis" file.   The simulation code starts by
> reading the mesh model from the "Genesis" file and initializes a new
> Exodus-II-formatted file with the mesh model in it and follows by writing
> simulation results to it.
>
> |Genesis File| --> |Simulation Code| --> |Exodus File| --> |ParaView|
>
> The "blocks" in an Exodus-II file are element-blocks.  In the original
> concept (and most software that uses the Exodus-II format), the finite
> elements in the block all possess the same geometry, same nodalization, same
> material model, and same element formulation (gradient & divergence operator
> construction).  In the simulation software, the the outside-loop is on
> blocks and the inside-loop is on the elements in the block.  A homogeneous
> domain can be processed as one block, or be sub-divided into any number of
> blocks in anticipation of post processing needs.  For a simulation code
> writing an Exodus-II formatted file, the blocks do not have to be
> homogeneous with respect to material model and formulation for ParaView.
>
>
>
> The Exodus-II format also supports hierarchical collections of element
> blocks that can be used for identifying "parts" or "assemblies of parts."
> However, the simulation code that writes the file needs to have this
> "knowledge."
>
> *EnSight.*  The EnSight format supports a concept of "parts."  Essentially,
> it is the idea of individual displayable graphics objects each with
> point-data and cell-data.  It is written out as if it were one large
> assembly.  ParaView via the filter 'Extract Block' can collect just those
> "parts" (1 or more) you want to view as a single item.  (I use the "part"
> feature extensively including writing out side-sets, node-sets, and other
> grid-sets that the simulation software knows about.)
>
> These two results file formats are quite flexible and allow you to use
> ParaView in rather amazing ways.
>
> Sam Key
>
> Rafael Castaneda wrote:
>
> Hi,
>
> thanks for answering. I've programmed a plugin for CFD preprocessing
> purposes (I mean, setting boundary and initial conditions, solver parameters
> and so on) and I would like that a user could make a model+mesh in ICEM CFD
> and export it to ParaView. When using ICEM CFD, one usually creates parts,
> which are grouping of 2D geometric entities, so that one can distinguish
> between different regions to attribute different BC's or IC's. The user also
> must create a domain, which is actually the 3D physical domain in which
> there is a flow.
>
> When I export to exodus II format, just the 3D Physical Domain is created
> as a block in the Multiblock Dataset, the 2D geometric entities, the parts,
> are not created. But I really need this information, so that I can
> distinguish the parts of the Model in my plugin and allow the user to select
> them to associate conditions. I tried exporting to fluent format in ICEM
> CFD, then opening with Fluent, saving as .cas file (which ParaView can
> read), but also: no information about the parts.
>
> The question is: is there any format or reader, available in VTK or
> ParaView that is known to read ICEM CFD Meshes with ALL the information ?
> I'm pretty sure someone somewhere already needed this !
>
> Thanks a lot for your help,
> Rafael Castaneda.
>
> 2010/1/19 Berk Geveci <berk.geveci at kitware.com>
>
>> Out of curiosity, what is the difference between parts and blocks? Or
>> are you using them
>> interchangeably?
>>
>>
>> On Mon, Jan 18, 2010 at 11:28 AM, Rafael Castaneda <ramacaneto at gmail.com>
>> wrote:
>> > Hi,
>> >
>> > I'm trying to export a mesh generated in ICEM CFD to ParaView. I
>> realized
>> > that I can export the mesh to Exodus II format and then open it with
>> > ParaView, but no information about the parts of the mesh is loaded, just
>> the
>> > blocks.
>> >
>> > Any reader available to export geometry and mesh from ICEM CFD to
>> ParaView ?
>> > I would like that the MultiBlockDataSet generated as result have
>> information
>> > about the parts created in ICEM CFD.
>> >
>> > Regards,
>> > Castaneda.
>> >
>>  > _______________________________________________
>> > 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
>> >
>> >
>>
>
> ------------------------------
>
> _______________________________________________
> 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
>
>
-------------- next part --------------
An HTML attachment was scrubbed...
URL: <http://www.paraview.org/pipermail/paraview/attachments/20100121/4a0148eb/attachment-0001.htm>