Hey guys!

As we know that you may either import the geometry or the shell mesh from any CAD package into STARCD. I created my geometry in IDEAS and transported the same. The problem I am facing is that I need to map 2 curved blocks. Mapping of a block face on a shell mesh can be done but since I do not have the shell mesh to begin with ( just the geometry) , I do not know how to proceed. If not remedied now, I might not be able to arbitrary mesh the 2 blocks as there will be problems with conectivity and voids will be there. Please help! Regards, Gurpreet

I'm not sure I understand your problem, but can't you use the "livesurf" command to create a shell surface of your geometry and map to that?

Hey Steve,

I will try using that command. I am actually trying to map a curved face block with a flat face block. I actually figured a way out for that without creating the shell mesh. I have a quick basic question though. Is it necessary to remove all errors like warpage , cracks before proceeding with the simulation or does prostar take care of it. I am not getting any of these major errors though : double vertices. negative volumes , overlaps.

what value of warp angle should we specify in general.

Its almost impossible to give an absolute number for a warpage limit. Cells with high warpage may do fine in one area, where nothing much is happening and the gradients are low, and still fail if located somewhere else - particularly nearer the surface. In the end, the only test that really counts is whether STAR converges or not. I suppose the basic answer is that it is not 100% required to get rid of every last shape problem (shape meaning, warpage, aspect ratio, internal angles...). Topology problems (cracks) don't have to be fixed either, but then if you don't, you won't be solving the problem you think you are. Cracks in the mesh introduce extra internal walls. Steve

Thanks a ton Steve. That should certainly help.

..I will be using the conjugate heat transfer model for my simulation and was wondering if we need to connect the solid and the liquid meshes too for the heat transfer part to run. In other words , will there not be a problem for the HT calculations if the solid and liquid meshes are not connected ( integral. arbitrary..).

Thanks again.

Yes - you do have to connect the solid and fluid. Thats how they transfer heat between them. However, it is OK to do it via cpmatching. Integral is safer, but arbitrary is also allowed with certain restrictions (it gets confused if you have a single fluid face attached to solids, other fluids and exterior walls all at one time)

Steve

Hey guys, Could some one please help me out with this one. Can we create a surface mesh (using livesurf) for a BLOCK only. The livesurf command asks for the cell set for which the surface needs to be created. For a block there are NO CELLS.... Otherwise I need to create the solid mesh for my block first and then generate the surface for that block.

Thanks

Gurpreet Gambhir

Sorry - livesurf only works on cell surfaces, not blocks. You would have to mesh the blocks to use it. You could use a very coarse mesh, but you do have to mesh them.

Hi guys:

I have a lot of vertices in my model which are redundant. They were created while I was generating a course mesh. I had to delete those cells later, but the vertices associated still remain. Would it pose a problem in the solution or do I need to delete all of them.

Thanks

Gurpreet

gurpreet,

Lot of vertices may cause sizing problems (if your computer resources are limited). Better to remove them by

cset all vset news cset vset inverse vdele vset vcompress all

ram