STL file for snappyHexMesh
 

Hi All,

I need to create a mesh by using snappyHexMesh.
I create the CAD file as an assembly and convert it into an STL. When I open such STL file it contains only a single "solid", while it should be composed by two solids, i.e. wall and cylinder. In this way I cannot distinguish them as different patches while making the mesh.
Does anyone know how to generate an STL file (from CAD) which contains the parts as different solids and not as a single object?
Best,

Tommy

Hi Tommy,

What you usually want to do is (1) to export the differet parts of your geometry in different STL files and (2) combine them in a single STL file and use it in snappyHexMesh.

1. Open the STL files with a text editor and check that the name of the boundary is correct. E.g.:

instead of
You change it into
2. Then you can combine the different STL files into a single one with:

Now you can access all your patches in snappyHexMesh.

Best,
Petros

hello tommy,
it depends in what CAD software you are using, from what I know, salomé, and blender (for sure) and maybe freecad? can do this.
if you are working with a different cad software than the ones i mentioned before, you have two possibilities (i recomend the fist one):
1. export your file (the complete geometry) in STEP format, import it to salomé (in the geometry section) and from there create groups with the faces that you want to be differentiated and then mesh it with 2D meshes, separatly, export them in separate stls and then use the command cat to create a combined stl. this way snappy will recognize the different groups you created. a good guide https://www.youtube.com/watch?v=CeuF...el=HolzmannCFD

2. use topoSet after doing the snappy by selecting the desired group of faces, the problem with this is that you are not going to be able to add the boundary layer in a specific patch. https://www.youtube.com/watch?v=l_ea...hannel=TheoOng

also recommend you to read the pinned post Creating waterproof STL using snappyHexMesh or salome

good luck!
franco

Hi Petros,
I did not think about it but your solution is very simple and smart.
Thank you very much for the tip!
Best,

Tommy

Hi Franco,
I use Autodesk Inventor and SolidWorks. Anyway, as far as I know, Salome and Blender are free, so I can consider to download one of them.
The solution suggested by Petros is great but things could come to be complex when you are modelling an assembly composed by tens of parts (at the moment it is not my case), and an automatic way to generate solids in the same STL could be very useful.
Thanks!

Tommy

hello tommyM,
the problem with petros way, and it really depends in the software (i dont know with solidworks and autodesk) is that when you do this without previously doing a remeshing of the surface you risk that your STL is not watertight. thats why you go to salome to remeshed and then export it separatly . please have a look at this post https://www.cfd-online.com/Forums/op...sh-salome.html

thats why i was telling you to go thought salomé, but you can try actually to export your different patches (in ASCII stl format!!!)directly from the cad software and use cat command ( you place all the stls in same folder, you modify them with a text editor and change the names as petros said, and then use the command (cat *.stl >> completeModel.stl). actually it is the same workflow as doing the salome path but the difference is that depending on the software where you export it, it is or not going to be watertight. and there you are going to have a only stl file (completeModel.stl) that it is going to have the boundaries (you should name them in the snappyHexDict too)
franco.

Franco is right. When I wrote my first post I assumed that the geometry is exported from a mesher like Salome or Blender. And by the way, you can always import CAD files into these software for manipulation.

Petros

Hi,
ok, I will learn to use Salome.
Thank you both for your hints, they are very helpful!
Best,

Tommy

I generally use FreeCAD with their mesh option, to export my stl files. Which if you are a solidworks user you pretty get familiar with.

STL file
 

Hello everyone

I export an STL file from surface Evolution to use for snappyHexMesh. Unfortunately, after running the snappyHexMesh command, it does not recognize the STL file and it is only show blockmesh in the form of rectangular channel.

Could you please help me how to proceed with that?

The problem is that you are doing things wrong:

code snippets from snappyHexMeshDict
You renamed you STL in the geometry section to be named interface. Hence, snappy don't know any guy named interface.stl. That's your problem. If you check the output of snappy, it will let you know:
It states, that the entry interface.stl is not used as snappy cannot find it.

Hi Tobi,

I am Lakshmi, from India. I am currently working on modeling a packed bed reactor for non-particulate systems. I wanted to contact you to know how to use OpenFOAM for meshing a packed bed geometry as I came across your discussions on this forum. I created my bed using blender 3D software and I shall export the geometry in the .stl format. I successfully created a blockmesh and I and facing the following error for snappyHexMesh (FOAM FATAL IO ERROR:
keyword locationInMesh is undefined in dictionary "/home/hp/OpenFOAM/hp-9/run/testcase_1/system/snappyHexMeshDict/castellatedMeshControls" ). Kindly help me if you know how to resolve this error. Looking forward to hearing from you. Thank you.

Regards,
Lakshmi

/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 9
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class dictionary;
object snappyHexMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

#includeEtc "caseDicts/mesh/generation/snappyHexMeshDict.cfg"

castellatedMesh on;
snap off;
addLayers off;



geometry
{
fluid
{
type triSurfaceMesh;
file "mesh.stl";
regions
{
wall { name wall; }
obj1 { name obj1; }
obj2 { name obj2; }
obj3 { name obj3; }
obj4 { name obj4; }
}
}
}

castellatedMeshControls
{
features
(
// { file "CAD.eMesh"; level 1; }
);

refinementSurfaces

{
#include "meshQualityDict"
fluid
{
level (0 0)
regions{
wall { level (0 0); patchInfo { type wall; } }
obj1 { level (1 1); patchInfo { type wall; } }
obj2 { level (1 1); patchInfo { type wall; } }
obj3 { level (1 1); patchInfo { type wall; } }
obj4 { level (1 1); patchInfo { type wall; } }
}
}
}

refinementRegions
{

}

locationInMesh (-1 -1 -1); // Offset from (0 0 0) to avoid
// coinciding with face or edge
nCellsBetweenLevels 1;
}

snapControls
{
// explicitFeatureSnap true;
// implicitFeatureSnap false;
}

addLayersControls
{
layers
{
"CAD.*"
{
nSurfaceLayers 2;
}
}

relativeSizes true; // false, usually with firstLayerThickness
expansionRatio 1.2;
finalLayerThickness 0.5;
minThickness 1e-3;
// firstLayerThickness 0.01;

// maxThicknessToMedialRatio 0.6;
}

writeFlags
(
// scalarLevels
layerSets
layerFields
);

meshQualityControls

{

#include "meshQualityDict"

maxNonOrtho 65;

maxBoundarySkewness 20;

maxInternalSkewness 4;

maxConcave 80;

minFlatness 0.5;

minVol 1e-13;

minTetQuality 1e-9;

minArea -1;

minTwist 0.02;

minDeterminant 0.001;

minFaceWeight 0.02;

minVolRatio 0.01;

minTriangleTwist -1;



// Advanced



nSmoothScale 4;

errorReduction 0.75;

}


mergeTolerance 1e-6;

// ************************************************** *********************** //