I am analysing the flow over a solid body which i want to rotate. When i create the mesh from pro-am a "cavity" is created where the object is. Is there any way in which i can mesh the object as a solid with a fluid domain around it so i can add rotation?

Hi Joel: You can define the surface between the fluid and solid as a rotating wall boundary in a csys to simulate the roating object. If you really need fill the cavity, use the "live surface" command on the fluid cells to create shells, then you are able to select the a closed shell that defines the solid domain. Cutting the selected shell in proam should give you the cells inside the cavity.

regards, ccy

cheers for that, i have tried the rotating wall i just never thought that it would be reliable as a rotating mesh but if it is it certainly a lot easier. The only problem is selecting all the walls as it is a complex geometry, is there a way of selcting all sufraces and then deleting as required?

Try the following:

cset,news,fluid live,surf (create shell type 100, for example) cset,news,type,100 vset,news,edge ctable,101,shell,3 cfin,shell,101,vx (then click a vertice on the outside surface) cplot (you will see the live surface has been separated into two different cell types, 100(red) and 101 (green)) cset,news,type,100 cfin,shell,101,vx (click a vertice on the outside surface) cplot ...

in this way,you modify unwanted shells to type 101. ===================

or if the bc's have been defined,try the following:

cset,news,fluid live,surf bset,news,region,1 vset,news,bset cset,news,type,100 cset,subs,vset,all ctab,101,shel,3 cmod,cset ...

BTW, solid cells are not counted in the calculation unless you are solving conjugate heat transfer problems.

Good Luck!

ccy

or if you have CAD data for the solid domain, then try the "pmap" command after "live surf". it will modify "live surf" cells that are close to the CAD data to the same cell type or by a offset.

regards, ccy

Cheers for that, one final thing (sorry you seem to know your stuff so i will bend your ear one last time). When i am refining my mesh i can refine surfaces easily but if i want to refine further than the surface how do i do that? By which i mean have a certain cell size close to the object, then getting larger further out. I read in the pro-am manual about the ccut comand but the section is very brief and doesnt really explain anything, in fact it says that further detail will be given in later versions!! in my model i need a fairly large domain so in the outer reaches i can afford reasonably big cells to reduce computational time but finer mesh close in.

Say if you want the cell size near the surface to be 2mm, for example, you can start building a mesh with a cell size of 8 mm. you put the mesh into a database as the custom mesh. Do classification, you are able to select the classified cells and refine them 2x2x2. put the refined mesh into a news database as the custom mesh and do the classification again. refine the the classified cells by 2x2x2, then you have cells of 2mm and 4mm near the surface and 8mm away from the surface.

ccy