# [ICEM] Meshing one body part only

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

 June 25, 2010, 17:21 Meshing one body part only #1 New Member   Join Date: Jun 2010 Posts: 20 Rep Power: 7 Hi all, I am new to this forum, and although I have some CFD experience, I just started using ANSYS. I have an assembly imported into ICEM, which is a enclousre containing some parts. The air inside the enclosure was identified by ICEM and a body part was created. When I do the meshing for the entire model, the air volume gets meshed, but it takes too much time, and I have to delete volume meshes for parts I don't need afterwards. The question I have is as follows: Is there a way for me to mesh the air volume only, without meshing the entire model? Any help would be appreciated.

 June 28, 2010, 14:23 #2 New Member   Join Date: Jun 2010 Posts: 20 Rep Power: 7 Perhaps, as an alternative, someone could suggest a way to refine mesh in one volume mesh block only.

 June 29, 2010, 11:37 Octree algorithm #3 Senior Member     Simon Pereira Join Date: Mar 2009 Location: Ann Arbor, MI Posts: 2,662 Blog Entries: 1 Rep Power: 35 Sometimes it helps to understand how the various algorithms work. The octree algorithm meshes the entire volume from min to max without respect to the geometry. The refinement algorithm is an OCTREE one that simply looks within each hexa and says "are there any entities within this box that are smaller than this current size. If yes, then refine (cut in half in 3 directions, 2^3=8, Octree). It refines inside and outside your area of interest based on your max size settings and any other geometry you have laying around. Then when all the refinement has stopped, it converts to tetra and transitions between mesh sizes. Then it fits to the geometry using the edge criterion to decide if edges need to be split before nodes can be moved to the surface (the message window will say it is running the "cutter"). Then shells are formed on the surfaces. Then the flood fill process happens. During flood fill, the algorithm finds a material point and marks it as in that part (such as FLUID), then it adds all the neighbor volume elements and continues until it is bounded by shells. (if a shell has the same fluid on both sides and is not marked as internal wall, it is removed, if the flood fill can go from the material point to another material point (such as the automatically created ORFN point outside the model), then you have leakage). After going thru each material point and flood filling, it throws away the remaining mesh and then it moves on to smoothing. In your case, you have no material points, so it helps you by creating one in each volume. If you manually create a single material point in your fluid region, it will prevent the other regions from filling, but it won't prevent the refinement, that is the inherent downside in the octree method. You could reduce your refinement by setting larger mesh sizes on the parts not adjacent to the fluid region you are interested in. Deleting geometry is also a good idea. If you mesh is good quality, you could try the patch dependent surface mesher followed by one of the bottom up tetra methods (such as Delaunay or Advancing Front). These have the advantage of being more targeted and only generating the mesh that you want, but the mesh setup is harder. If your geometry is relatively simple (topologically speaking), it may be best to generate a quick Hexa mesh on it. For instance, an exhaust assembly may create quite a large box in XYZ space, and so would be very inefficient for octree tetra (unless you meshed it in smaller segments and merged them). However, it is relatively simple topologically and could be very easily hexa meshed. Post an image and I can make a custom suggestion.

 June 29, 2010, 15:36 #4 New Member   Join Date: Jun 2010 Posts: 20 Rep Power: 7 Thank you for the detailed explanation! This helps a lot. I will try to remove material points from all bodies except the air volume. This way only the mesh which connects to material points will be left during the flood, if I understood correctly how the process works.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post mahadevan.swamy Main CFD Forum 1 June 23, 2009 10:13 qascapri ANSYS Meshing & Geometry 3 May 22, 2009 12:46 Farhat FLUENT 0 May 27, 2007 00:08 rai FLUENT 0 December 19, 2005 01:46 Manoj Kumar FLUENT 0 June 20, 2005 01:02

All times are GMT -4. The time now is 06:48.