Error: No Triangles in Surface
 

"Error: No Triangles in Surface"

Pretty new to CFD, have a very basic understanding of some stuff, but utterly stumped by this error message. Appears when I try to generate a volume mesh using the Trimmer and Surface Remesher on a fairly complex geometry designed in Star (not imported)

Scanned here and the internet, as well as the help files trying to at least find out what it might even mean, let alone how to solve it!

Tried rolling back the model to see what is causing the issue, but as soon as I do that it fires up saying the "Surface is not Closed"

Driving me slightly mental, so any help would be greatly appreciated!

Cheers

Oh well
 

Ok, never mind, I've started again and got it working

Mods, feel free to delete this thread.

Hi Saxon,

this issue typically occurs when you make a "mistake" with the initialization of the meshing.
Just imagine, you've got one geometry part assigned to a region. When you press the "Initialize meshing" button, the geometry is transfered to the initial surface representation. All is fine.
Now you'll delete the assignement of the part to the region (let's say you've allready created a volume mesh, but forgott to split some boundaries). Create a second part and a second region and press "initialize meshing" again.
It will transfer the geometry of the second part to the initial surface representation, but will delete all faces from the first region.

So you don't have an initial surface representation for all regions.

Better to create all needed regions BEFORE initialize meshing, and all is fine.

Good luck

Hi Abdul (or anyone else that can help me), i've got the same error message, and can't work it out. I'll explain my problem.

I've got a wind turbine made up of only three blades. I have analyzed it importing (from solidworks) the blades as Parts, then in Star i've created two other Parts: a cylinder that contains the blades and that will simulate rotation, and a large block to simulate the stationary air all around (that contains the cylinder and the blades, of course).
I've then assigned them to two regions, "rotating" (cylinder-blades), and "stationary" (whose sides are inlet and outlet and slip-walls) with an Interface between them.

I've runned the simulation without problems. Now i need to substitute the blades with others, always from Solidworks, and here come the troubles. How i'm supposed to do this?
First of all, i've cleaned up the solution and the mesh. Then i've imported the new blades as parts, and deleted the old blades (from Parts and from region "rotating"). Then assigned the new blades to the region. Then tried to create a new surface mesh. Here i've got the error message about triangles, but from "stationary" region...!

Im new to cfd, so forgive my errors. Any help will be appreciated. thanks.

Not really sure what you did. My first idea is a "split by surface topology" on region level which could cause the problem, because there is no longer a part surface assigned to a boundary. You do not only need to assign a part to a region, you also have to assign part surfaces to a boundary (pretty much the same way like assign a part to a region). Otherwise the surface remesher will find the boundary but don't know it has to transfer the geometry to the boundary - and therefor can't find any triangles in the surface.

Usually I prepare my geometry by doing boolean operation on part level. When I create regions, I've already finished ALL geometry preparations and the parts and assigned regions are exactly the geometry I want to solve the flow.
I recommend you to do the same, because afterwards you can import a new geometry, do the boolean stuff again (with the new rotor blades) and you just have to assing the new part surfaces to the old boundaries.
And with that approach, you don't have to split up anything on regions. You don't have to clear solution and mesh. The old solution will be mapped on the new mesh and you can get a converged solution on the new mesh much faster.

Cheers

you are absolutely right in what i did wrong (i've used Split by surface topology). also your tips are very useful.

i did some operations directly on regions because on part level i can't find out how, for example, use Split by angle (i had to do this for the external block, to split it on 6 boundaries to create flow inlet, outlet and so on).

now i've noticed that all my boundaries have no Part Surfaces assigned in their properties box. is this due to the fact that i've operated directly on regions? is it an error? the simulation run anyway and the results seems good.

I've however already created new simulations using different approaches. i'm new to star-ccm (and to cfd) and i'm learning new things every day.

Thanks a lot for the reply :)
Cheers

The list of things you can do on part level is increasing with every new version of star-ccm+. Split by angle should be possible since v5.02 or v5.04.

Your boundaries don't have any part surfaces assigned due to the split by surface topology. You've got a message, that all assignements will be deleted, haven't you? It might be annoying to the user, but it's not an error.

Good luck for further work!