Was just playing with solid elements and tried to do a simple analysis of a solid cylinder fixed on one end and subjected to an axial load on the other end.
I wanted Hex mesh on the entire solid. So I created a surface quad mesh seed on one of the face of the cylinder with elements with no attributes as shown below
I created a solid property and I used the option Mesh->Geometry->Hexmesh Solids. The mesh appears alright but the color is red (which I assume means something wrong) and also an error message "Solid1 cannot be Hex meshed. Meshes on base & top surfaces do not match". I don't understand this error message. I've seen elsewhere solid cylinders being Hexmeshed using the above procedure.
Just for the heck of it, I tried meshing the solid using Tet elements and I was able to run the analysis successfully.
Would appreciate some help on debugging.
Solved! Go to Solution.
That's exactly the error message you have: your mesh at top & bottom is not the same, then impossible to create a HEX mesh. The HEX mesh command in FEMAP runs like an extrusion, then if both 2-D surfaces meshes at top & bottom are not exactly the same, them the error FOR SURE.
You can make the 2-D Surface mesh yourself using a PLOT-ONLY 2-D mesh, if not FEMAP will do for you internally: during the process of hex sizing using command MESH > MESH CONTROL > SIZE ON SOLID, FEMAP identifies the base and top surfaces and automatically matches (slaves) the mesh on the two surfaces. This is required for successful hex meshing. The base and top surfaces must produce the same surface mesh, not necessarily the same shape, but the same number of nodes and elements with the same connectivity.
The lateral or side surfaces (everything but base and top) control the mesh “along the length” of the extrusion. You can avoid using command MESH > MESH CONTROL > SIZE ON SOLID, simply do a 2-D PLOT-only mesh (not attributes) of the full cylinder making sure you use a CONSTANT ELEMENT SIZE between top & bottom, OK?. (exactly the same element divisions in top & bottom surfaces).
Next use command MESH > GEOMETRY > HEX MESH SOLIDS and you are done!!. This is easy, but first you need to understand how FEMAP runs internally, simply, like us!!.
The method you proposed i.e. to generate 2D mesh on all surfaces using plot only elements, did not work as expected.
Femap is creating slightly different mesh on top & bottom surfaces of the cylinder. So using Geo->Solid->Hexmesh is not working.
Pls take a look at the image below. Right in the center (highlighted) by red circle, the elements on both faces are not matching.
However, I was able to get solid mesh using Extrude command but I am interested in generating a hex solid mesh using Geo->Solid->Hexmesh command.
The only other way I can think of is to copy the seed surface mesh from one face to the other but I don't know how to associate the copied mesh with the other surface.
Anyways, I would appreciate if you could try out your propsed procedure and provide detailed instructions or illustrations on how you accomplished.
Thanks for replying. I apprecaite your efforts...
If you run the correct workflow in general you will success:
The above procedure works OK with regular geometries, if the geometry is complex you will need to slice the solid to create regular bodies. Go to my blog and do a SEARCH for HEX MESHING, you have videos and different HEX meshing procedures explaining how to do tricked hex meshing in FEMAP, ok?.
You might need to check that one of the end surfaces is "linked" to the surface at the other end. This is set or checked using Mesh -> Mesh Control -> Approach on Surface. Check this at both ends. If there is no Master / Slave relationship, then set one. If there is a Master / Slave relationship, try it switched off. Delete all surface/solid mesh on the cylinder before retrying the hex mesh operation after setting or deleting the Master / Slave relationship on the end surfaces.
You can associate a copied (or extruded) mesh using Modify -> Associativity -> Automatic.
Finally, once you get the top / bottom (ie. circular ends) meshes matched, you can use Mesh -> Geometry -> Hex Mesh from Elements.
Amongst these, you will get an associated hex mesh on the cylinder. If not, then there is a non-visible topology problem with the cylinder - eg. something like 4 edge curves used to define one circular end, but two edge curves used to define the other circular end.
I have to apologize here, especially to Blas.
I was entering the size of element in Tet Mesh tab under Size on Solid and trying to Hex mesh it. I guess, thats why Femap was unable to produce a successful mesh.
I just realized it now and I am able to obtain a Hex Mesh of the solid cylinder.
Thanks again for all the folks who have replied. My bad on starting this topic.