[Sam0508]

How to choose the right Mesh base size value from the model.let we take an eg of fluid flow area is 1mx0.5mx0.3m.
What will be Effect of target size in this state? how to find these value?plz any one can give guidelines



Regards,
Sam

[willimanili]

The idea behind the base size is, that you can set other values like surface minimum / target size, boundary layer thickness e.g. proportionally to the base value. So if you like to refine or coarsen your mesh you just have to change the base size value. All other values which are defined by the ratio to the base size will change automatically. If this feature is really helpful to you you have to decide by your own. I use absolute values mostly, especially for the boundary layers.

The target size is the maximum face size for the remeshing process. The minimum size is like the name already said the minimum face size. The remesher will always try to mesh the surfaces with the target size if not other settings force him to refine the mesh at certain locations. But the remesher wont use faces smaller than the minimum face size. So with this values you can specify how fine your surface mesh will be and how strong the remesher will refine the mesh if it is necessary.

[Sam0508]

Hi willimanili,
Thankyou for ur reply

[Sam0508]

Hi willimanili,
1.When we useSurface wrapper option and need?

2.Do u have an idea about porous medium if yes how to find tha Alpha and Beta value in STAR CCM+ simulation.

Thanx in adv


Cheers,
Sam

[madhuvc]

say you are starting from poor CAD and if you dont want to manually clean the surface , you can use surface wrapper. It gives you a closed non-manifold surface which can be used for surface meshing. Surface wrapper needs to be used with caution, since the extracted geometry can be of no use if you use the wrong parameters. It needs some practice. the good thing is if you how to use it, it can save your time in cleaning up the CAD. you need to select both surface wrapper and surface remesher models to have a volume meshable surface mesh.

it can be used to clean baffles, fill holes and gaps, extract required geometry from a complicated part etc.

[madhuvc]

for porous medium alpha and beta values ,
i guess you have experiment/test values for pressure drop & flow rate. if you have those values you can plot DelP/unit length and velocity. if you line fit the graph (Right click on the plot in excel --add a trendline) into a quadratic function, the values you have are those for inertial and viscous resistance. please make a note no inverse values are required as in FLUENT. you need to find out what kind of resistance you have isotropic/ orthotropic ...

[Sam0508]

Thankyou...

[Sam0508]

Is it possible to do without experiment pr drop value? i.e i want get value frm STAR CCM+ itselt...what is the procedure?

[LuckyTran]

Originally Posted by Sam0508

Is it possible to do without experiment pr drop value? i.e i want get value frm STAR CCM+ itselt...what is the procedure?

No. Star-CCM is not used for deriving new physics of porous media, it simply uses the Darcy model or derivatives of it. Star-CCM is designed to let you solve the resulting flow field assuming you already know how the porous media behaves.

There are correlations for what the alpha and beta values are for packed beds and some other situations but again, you must know alpha and beta somehow, Star-CCM will not calculate them for you.

[kamillaa]

I have a short question, what is the minimum size of a lenght/width in Star-CCM+? I have simulated a film (oil layer) with the size 1mmx100mm and want to decrease the height to e.g. 0.5mm or even 0.9mm if possible, but the program refuses to change the size... Is 1mm the lower limit?


Edit: Forget about it! It seemed to work when I created a new file... Thanks anyway!

[jhv_1729]

Originally Posted by Sam0508

Is it possible to do without experiment pr drop value? i.e i want get value frm STAR CCM+ itselt...what is the procedure?

If you have the specifications of the porous medium like the velocity through the medium vs pressure drop you can convert it into the form of equation shown in the user manual using a simple curve fit.

You'll have to experiment if you don't have the specs.