i am a beginner in use of starcd,I need a tutorial that takes a model from importing iges, through pro-surf, through pro-am, to pro-star boundary setup and the different cell type setup to running etc,can u give me some advice?

thanks

elvis

dude,

this is the path i take,

i dont have a tutorial that i could give you,

the easiest way is to just try it out for youself,

or

following the tutorials in the manuals

there are pro-surf and pro-am tutorials in the documentation.

thanks a lot for your suggestion,but if I want to simulate a double pipe heat exchanger. i design the model in solidworks,and saved as *.iges,then follow with the path i given, how to deal with the outer wall , annular fluid, inner wall (finite thickness) and inner fluid? especially about how to deal with the thickness of the wall because i want to use it for heat exchange.somebody say set it to solid cell,but how set when have meshed in proam? Just give me a outline.

thanks again

elvis

sorry dude, you need to contact you local Adapco support for help, i'm not sure the best approach to model a double pipe heat xchanger

I can't help with prosurf (I've never used it), but I would suggest three ways to create the volume mesh in proam.

1) There is an option to include interior baffles in the meshing process. You have to define the walls of the inner solid as a seperate cell type (you can use Tools -> Cell Tool for this purpose) and follow the instructions in the proam manual for mesh generation. You should get three disconnected regions, therefore it will be easy to define materials for the different cells (again with the Cell tool). After you have defined your cells, you have to merge the vertices (command: vmerge).Unfortunately, this approach will only work for tet-meshes, which might cause a problem if your solid is very thin.

2) The other possibility is to mesh your fluid volumes first and then create shells on the two seperate volumes (command: live surf or Add Shells in Cell Tool). Then you can extrude (using vcextrude) from the shells on your solid wall to create your solid volume (with prism or hex cells). This way you can avoid creating loads of tetrahedral cells in your solid, but it can be quite tricky to get a working mesh. The problem is you will have to create couples on a non-planar surface (not very easy to do). I usually do the following: I first extrude the two shell sets (i.e. the two solid walls) inwards to create volume cells with a gap between them. Next create shells on the inward faces of one of these volume cells and project the vertices of the inward faces of the other cells onto these shells (command: vpro). Afterwards you have to create couples between these cells (you can use the couples tool for this purpose). This approach has the advantage that you have one-to-one connectivity between your fluid and your solid cells. If you try this way as a beginner, be prepared for some rather frustrating time...

3) If you have straight pipes I would just create a section through your pipe and extrude it without bothering about a closed surface.

I hope this didn't confuse matters even more and will help a bit.

Good luck,

Volker

thank u very much,ok,i think i am interested in the first way given by Mr. Volker,and i will try it again.but i still have some quetions about the model,we know,we calculate the volume about fluid or the solid(if have heat transfer) in cfd,but we design the object in cad only the solid figure about the model ,how can i get the fluid part,in cad or proam?

thanks again,u are so kind!

elvis

Elvis,

I understand your problem now (I think). You need to have closed surfaces for all your different materials. These include the solid surfaces that enclose your fluid as well as the inlets and outlets where no physical boundary can be found. In your case they are two fluid volumes and the solid volume (obviously some of the surfaces are used for both solid and one fluid volume). Therefore, you either have to generate a CAD model that includes all these surfaces or add them to your existing model. I have never used prosurf (we use ANSA), but I would imagine that you can add surfaces with it.

When you get 'raw' CAD-data of a given part or device, you will probably spend quite some time cleaning your surface until you have something that you want to use as a basis for your volume mesh (e.g. deleting surfaces that you don't need, adding surfaces, simplyfying the geometry etc.).

Good luck,

Volker