CFD Online Discussion Forums

CFD Online Discussion Forums (
-   Siemens (
-   -   no boundary on shell (

Ted Crilly March 15, 2005 18:49

no boundary on shell
hi there,

quick one, when you have a shell that has no boundary defined on the shell, what does it default to?

thanks for any advices


carno March 16, 2005 02:09

Re: no boundary on shell
shells do not participate in computations. So no question of BCs.

Ted Crilly March 16, 2005 08:49

Re: no boundary on shell
so they are treated as adiabatic surface?

if i assign an inlet to a shell, it definately does participate in the computation

for example if i use live,surf on subsurface created by pro-am but dont define a boundary on the shells, what are they treated as? adiabatic surfaces?

Jörn Beilke March 16, 2005 13:26

Re: no boundary on shell
Shells are only used for pre and postprocessing. If you want then in the solutiuon you have to use baffles.

Ted Crilly March 16, 2005 18:50

Re: no boundary on shell
hi jorn,

i'm not sure if we are talking about the same thing,

when i generate a mesh in pro-am i get it to generate boundary shells for all the surfaces, it does this for all the surfaces in the model, subsurface inner surfaces and no subsurface surfaces too.

so my cell table looks like this

1 fluid.... main fluid domain 2 solid ... nothing 3 baffle ... nothing 4 fluid .... subsurface fluid domain

5 shell ... floor surface 6 shell .... wall surface 7 shell .... ceiling surface etc etc

so the shells are already there,

alternatively i can use :

live,surf and create new shells on whatever surface i choose

Then in pre-processing i assign boundaries to these shells, so for example

cell table 5 shell - floor surface - wall fixed temp 293k etc etc

so i setup and apply boundaries to these shells,

some boundaries are setup as walls, some as inlets/outlet/pressure etcetc

obviously they are part of the solution, the heated floor is there in the solution the inlets blowing in 10ms-1 is there in the solution.

My question is how does Star-CD treat a surface that has shells applied to it but the boundaries have not been setup?

i.e. it knows its a solid boundary for example a wall or ceiling, but it does'nt know what temperature, velocity etc, what does it default to?

do you get my point

thanks for helping to try and clear this question up


Jörn Beilke March 16, 2005 19:43

Re: no boundary on shell
You apply the boundaries to the faces of the fluid cells!

For that purpose you might use the help of shells but this is just one way. Using the bcro or the bfin commands you can apply the boundaries to the cell faces without having a single shell in your model.

It seems that you have a completely wrong understanding of the concept of shells in star. The name field in the cell table is just a name and nothing else. You can also write a short poem there if it makes you happy :)

Ted Crilly March 17, 2005 07:56

Re: no boundary on shell
thanks, i will have to rtfm again,

dont worry, i'm well used to not getting a straight answer in this industry,

good day to you

Pauli March 17, 2005 09:51

Re: no boundary on shell
All boundaries of the fluid domain default to region 0. They will use the values you assign (or the defaults) of region 0 unless you define them otherwise.

From you description, it sounds like the fluid cell faces and the shells have coincident vertices. That is the key to it working.

Unless they provide some benefit in defining boundary regions, there is no need for the shells. I am pretty certain they will be ignored during the calculations.

Ted Crilly March 17, 2005 11:56

Re: no boundary on shell
thanks alot pauli,

keep up the good work

BV March 18, 2005 02:22

Re: no boundary on shell
Ted, Tell me how to get the bounadry shells for all surface seperately(as seperate entities in cell table)and assign boundaries to surfaces in PRO AM as u explained above.

Ted Crilly March 18, 2005 10:20

Re: no boundary on shell

in prosurf dont group trimmed surfaces together when importing iges, export surfaces as groups or individual surfaces if you like.

you need to generate mesh with pro-am, make sure under the advanced option (in generate mesh) you tick add boundary shells, when your complete assembly is made the shells are there.

The shells for any cell table with no subsurface are fine and can be used directly for assigning boundaries to.

But the cell tables that have a subsurface are setup with new shells on the inner face of the subsurface, when you really want them on the outer face and you need to manually do these ones again with, live,surf,create etc it can be a right pain

i'm sure there is an easier way to do this.

I need a tutorial that takes a model from importing iges, through pro-surf, through pro-am, to pro-star boundary setup to running etc, but there does'nt appear to be one


All times are GMT -4. The time now is 10:04.