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

Patran Volume Meshing

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 9, 2003, 04:58
Default Patran Volume Meshing
  #1
Deb
Guest
 
Posts: n/a
Hi all!

I have done a volume mesh with PATRAN VOLUME MESHING. But before exporting the mesh in a NEUTRAL PATRAN file, I must create "Patchs" to define surfaces on which I will apply boudaries conditions after importing the mesh in CFX Build (5.5.1). How can I define these patchs ?

Thanks in advance

Deb
  Reply With Quote

Old   April 9, 2003, 12:36
Default Re: Patran Volume Meshing
  #2
cfddoctor
Guest
 
Posts: n/a
you need create groups (of nodes) and export them
  Reply With Quote

Old   April 10, 2003, 03:30
Default Re: Patran Volume Meshing
  #3
Deb
Guest
 
Posts: n/a
Hi cfddoctor!

Yes, I have tried to create groups of nodes for 2D regions but I don't know how to do in Group/create...
  Reply With Quote

Old   April 10, 2003, 06:23
Default Re: Patran Volume Meshing
  #4
Louwrens
Guest
 
Posts: n/a
You have to select the nodes on each boundary that you want as a patch, and create a 2D group of that (Group -> create etc in 5.5.1)

You also have to select all your nodes and create a 3D group for the flow domain.

Good luck for selecting those boudnary nodes if they're not nicely aligned... I never found an easy way to do it!

L
  Reply With Quote

Old   April 10, 2003, 10:53
Default Re: Patran Volume Meshing
  #5
Robin
Guest
 
Posts: n/a
FYI

The handling of 2-D and 3-D regions when using the Patran volume meshing has been significantly improved for 5.6.

Doesn't help you much now, but it at least gives you something to look forward to.

Robin
  Reply With Quote

Old   April 10, 2003, 11:46
Default Re: Patran Volume Meshing
  #6
Robin
Guest
 
Posts: n/a
Hi Louwrens,

A trick I have found to work with not-so-nicely-aligned boudaries is to do the following:

1. create the volume mesh 2. add the surface to the group 3. hide all the nodes 4. transform the GROUP containing the surface by a distance of <0,0,0>

When you transform the surface, all the nodes associated with that surface will magically appear! Since you hid all the other nodes, you can simply box select the ones you need for the boundary region.

This only works if the nodes are associated with the surface. If the surface is a face of the solid you meshed, this will be done already. If you created the volume mesh by gliding along a path or rotating etc., you may have to manually associate the nodes to the surface.

Regards, Robin
  Reply With Quote

Old   April 10, 2003, 12:07
Default Re: Patran Volume Meshing
  #7
Bob
Guest
 
Posts: n/a
Robin, another useful tool for the picking of nodes is under view/scale factors. This can sometimes help but not always. usually helps if the geometry is simple but the mesh is real fine due to seeding near to the boundary. Bob
  Reply With Quote

Old   April 10, 2003, 12:09
Default Re: Patran Volume Meshing
  #8
Bob
Guest
 
Posts: n/a
Its a shame a surface mesh can not be placed on an object and its nodes used for the boundary group and then also used for the volume mesh definition. That would seam a quite simple approach ??? bob
  Reply With Quote

Old   April 10, 2003, 15:34
Default Re: Patran Volume Meshing
  #9
Sharks
Guest
 
Posts: n/a
Bob,

In CFX-5.6, the Patran Volume Meshing tools have been made much easier to use with regard to identifying regions.

The same 2D (surface) and 3D (solid) region forms used for native meshing are also used to allow selection of geometric objects rather than specifying groups of nodes.

The export of all the mesh and region data is handled automatically through a Write File icon (analagous to Write Definition File).

Regards,

Sharks
  Reply With Quote

Old   April 10, 2003, 15:41
Default Re: Patran Volume Meshing
  #10
Robin
Guest
 
Posts: n/a
Hi Bob,

You can certainly do that, just make sure you equivalence the nodes before writing the neutral file.

Robin
  Reply With Quote

Old   April 10, 2003, 22:10
Default Re: Patran Volume Meshing
  #11
Dany
Guest
 
Posts: n/a
Robin,

I'm quite curious if 5.6 will help me got rid of the unneccesary edges on the solid surface. You will be aware that the elements always gather at the edges, esp if the surface is curved. I import a set of mutliple surfaces to Build and then convert it to B-rep rather than a single solid surface(from CAD). Please advise. 5.6 is still a blackbox to me. Really hope you could add some functions to this.
  Reply With Quote

Old   April 11, 2003, 11:22
Default Re: Patran Volume Meshing
  #12
Robin
Guest
 
Posts: n/a
Hi Dany,

Are you referring to the unstructured meshing or Patran Volume Meshing?

Robin
  Reply With Quote

Old   April 11, 2003, 15:20
Default Re: Patran Volume Meshing
  #13
Dany
Guest
 
Posts: n/a
I'm referring to both structured & unstructured mesh. Can you please advise?

Thanks, Dany
  Reply With Quote

Old   April 11, 2003, 15:23
Default Re: Patran Volume Meshing
  #14
Robin
Guest
 
Posts: n/a
Dany,

On the unstructured side it's easy; simply create a merged surface. There are tutorials in the documentation on the use of the surface editor tools, or you can contact you support rep for more info.

Robin
  Reply With Quote

Old   April 14, 2003, 11:05
Default Re: Patran Volume Meshing
  #15
Bob
Guest
 
Posts: n/a
Robin, I thought that the structured surface mesh had no relation to the volume mesh ie node one of the surface mesh would not necessarily be in the same location as node 1 of the volume mesh. So are you saying this is not the case ? Also what happends when you equivalencee the nodes ? I've been instructed to equivalence the nodes at the volume meshing stage, before reading the mesh into the mesh import database. But if I created a surface mesh, copied those nodes into a group, then equivalenced, would my boundary nodes be all wrong ? Cheers Bob
  Reply With Quote

Old   April 14, 2003, 14:13
Default Re: Patran Volume Meshing
  #16
Robin
Guest
 
Posts: n/a
Hi Bob,

I did not say to create a surface mesh.

As for your question, a surface mesh may not have the same node distribution as the volume mesh.

Robin
  Reply With Quote

Old   April 14, 2003, 23:25
Default Re: Patran Volume Meshing
  #17
Dany
Guest
 
Posts: n/a
Robin, Can I simply merge all the surfaces together (for 3D curved diffuser)? Someone has told me before that merging surface on different plane in Build isn't a good idea. Please give some quick advice of whether it's true to say so.

Thanks, Dany
  Reply With Quote

Old   April 16, 2003, 15:13
Default Re: Patran Volume Meshing
  #18
Robin
Guest
 
Posts: n/a
Hi Dany,

You can merge them together if you do not need the boundaries. If the surfaces meet at a sharp edge, merging them will cause the mesher to ignore the edge, which is probably not what you want (although in some cases it may be desirable). Also, you cannot merge surfaces which are to be used in separate boundary conditions.

Robin
  Reply With Quote

Old   April 17, 2003, 00:22
Default Re: Patran Volume Meshing
  #19
Dany
Guest
 
Posts: n/a
Robin,

Are you referring to the common edges on the surfaces where the mesher will ignore?

Your info is quite useful for me.

Thanks, Dany
  Reply With Quote

Old   April 17, 2003, 10:56
Default Re: Patran Volume Meshing
  #20
Robin
Guest
 
Posts: n/a
Hi Dany,

Yes. Suppose you have a flat surface which is made up of several surface patches. By default, the mesher will resolve the edges of each surface, which may produce slightly poorer quality. The merged surface feature will use this mesh to create a new parameterization of the surface and will only resolve the outer edges of the surface (or inner edges if there are holes).

Where it really makes a difference is when you have a cusp. Suppose you have two surfaces which meet along an edge, one surface is square, but the other has a curve which meets the common edge at a tangent. The first surface is easily meshed, but the second will cause problems as the surface mesher has to reduce the angle to zero as it approaches the cusp. Physically, this feature does not exist. So to get around the problem, you can create a merged surface between the two. Where you previously had an angle of zero degrees, you now have a 90 degree angle, which is no problem to mesh.

Another use for merged surfaces is to "de-feature" the geometry. Suppose you have a surface with several small depressions where screws are intended to go. If you have determined that these do not have a significant effect on the flow, you may not want to mesh them. By default, the mesher will resolve all the edges and surfaces. If you create a merged surface, it will pave over the holes, ignoring the edges.

Other problems may occur where you have inflation off a surface which goes around a sharp corner. If the sharpness of the corner is not really important, you could merge the two surfaces together and the mesher will only resolve the edge within the local mesh length scale, but not try to put nodes exactly along the edge.

Last, but not least. A merged surface can overcome some shortcomings of the Advancing Front surface mesher. The AF surface mesher cannot mesh a closed surface, but the Delauney surface mesher can. If you have a closed surface and create a merged surface on it with the Delauney method, you can then switch to AF and mesh it as a merged surface. This is because the new "merged" topology is no longer parametrically periodic. Pretty cool!

Hope this helps.

Best regards, Robin
  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
Volume 1 has invalid topology for mapped brick meshing georgewar ANSYS 0 July 24, 2011 16:02
'Tetrahedral meshing has failed for volume...' Murat FLUENT 5 February 19, 2011 04:22
Error during volume meshing "Surface is not qualified for meshing" scorpionbay2 STAR-CCM+ 1 December 21, 2009 11:14
Gambit: Volume Meshing fluentnoob ANSYS Meshing & Geometry 4 May 20, 2009 05:21
meshing lubricant volume kenneth FLUENT 6 August 7, 2000 12:37


All times are GMT -4. The time now is 18:09.