Hello,
I am curious if someone may know how I can mesh this with brick elements and have through thickness mesh of approx 3-4 bricks. I have played around with it for a while and can’t seem to figure it out. It has to be a solid model due to checking plastic strain.
Hex meshes in PrePoMax can be generated by:
So you could split the component into parts that can be meshed by extrusion, revolution, or sweep (which may not be easy in some cases because, e.g., revolution has some additional limitations). However, it might be better (at least for the elliptical dome itself) to just split it in such a way that it can be meshed with the transfinite algorithm. Either way, later you can connect the pieces with tie constraints or the Merge Coincident Nodes tool.
Thanks, that looks exactly like I need. Is there a way to also specify through thickness node or element count?
With the Transfinite algorithm only via global (Meshing Parameters) or local (Mesh Refinement) element size definition. Direct specification of the number of elements/layers is only possible with the extrusion and revolution algorithm.
Another way you can often use to get nice hex meshes is to import a surface geometry, mesh it with quad elements and then use the Thicken Shell Mesh tool to offset it and create a hex mesh with a given number of layers. Here’s an example: 3D Interactive Analysis Stress Viewer - #11 by Matej
I’ll give these options a try. One thing is that the plastic strain will be checked at the nozzle/head junction which requires a very small fillet to avoid a singularity. With having separate parts, this could be an issue. I am assuming one workaround would be to make the nozzle hole in the head larger and add a set-in shell/fillet/nozzle part to tie constraint. Effectively bypassing this concern?
Tie constraints won’t be needed if you use compound parts and transfinite or thickened shell approach. Then the mesh will be continuous. Ties are only necessary if you use extruded/revolved meshes or want to connect meshes created in different ways.
You could also use a mixed mesh model (most of the head modeled as a shell and tied to a smaller solid region around the nozzle) or even submodeling - those are the most common techniques in such cases: https://youtu.be/RNVE1rk1yps?si=cYnqHLvKQa8zKqNt
It looks like the easiest way I did it was the thicken shell method. Do you have any tips for smoothing out this irregularity towards the nozzle, or does it really even matter?
In addition to the previous question, do you have any tips on alleviating this stress singularity at the nozzle junction? If I make everything a compound part it seems that I cannot assign a different thickness to the nozzle which is necessary. However, there is obviously a concentration here that is not real.
There are two ways to have more regular mesh with Gmsh - either partition the surface geometry (e.g. split the dome in 2 perpendicular planes) and make sure transfinite 3- and 4-sided faces are enabled in Gmsh shell meshing algorithm or use Quasi-structured Quad algorithm for Gmsh shell meshing.
Yeah, unfortunately, the Thicken Shell Mesh tool is applied to all surfaces if it’s a compound part. So you could leave some segments as separate parts and then tie them to the compound or merge the nodes if the meshes match (nodes have to coincide with a small tolerance).
But, as I’ve mentioned before, I would use shells for the majority of the model and solids only for the junction. Abaqus even has a special constraint for such cases:
Oh, and I forgot to say that you should utilize symmetry whenever possible and analyze a quarter of the head if its (full or simplified) geometry, BCs and loads are all entirely symmetric. You can often use axial symmetry in such cases too. Symmetries not only speed up the analysis but also make it much easier to apply boundary conditions and mesh the model with hexahedral elements.
For alleviating the stress in that area you should model also de weld bead, start with a straight chamfer and maybe add radius to the new edges. Probably it cannot meshed with hexa elements unless you made several partitions.
Here’s a nice example of partitioning and meshing for a fillet weld from a Polish book “Analiza konstrukcji walcowych zbiorników ciśnieniowych w strefach otworów” (Analysis of the cylindrical pressure vessel structures in opening zones) by A.P. Zieliński et al.:
There are also examples for a chamfer weld and some other special designs (including reinforcing pads).
I would make a 2D mesh like this (with fillets) and then spin it (quarter spin shown below)
That gives good mesh control.
Yes, this approach can also make it easier to define complex composite layups on detailed nozzle models. Abaqus even has a special keyword to revolve meshes and transfer results from axisymmetric to 3D models: https://classes.engineering.wustl.edu/2009/spring/mase5513/abaqus/docs/v6.6/books/usb/default.htm?startat=pt04ch10s03aus53.html
However, in PrePoMax, you can’t revolve an existing mesh like this so other tools have to be used (e.g. Gmsh). In PrePoMax, you start from a solid mesh, set 2D algorithm (it helps to partition the source face so that transfinite 3- and 4-sided faces are used - sweep also supports the Quasi-structured Quad algorithm) and the model is internally replaced by a revolved 3D mesh.
https://www.youtube.com/watch?v=1kOHe-GGCHM this tutorial gives a reasonable approximation to the method in PrePoMax, the auto-meshing features can often save time but sometimes won’t quite do it how you want. The pictures were made in LS-Preprep. I only work with composites BTW!
Yeah, that’s just what I meant. This feature (along with Extrude Mesh) uses Gmsh. In Gmsh, you start from a surface geometry and extrude/revolve it together with the mesh. I covered it before the PrePoMax implementation: https://youtu.be/f0bnLlQETgI?si=0k6nKKAiYONgu165
Now it’s implemented in PrePoMax in such a way that the imported CAD geometry is internally replaced by the result of Gmsh’s extrusion/revolution.
However, transfinite meshing (also using Gmsh) can be more versatile and helpful also in the cases such as pressure vessels with features that aren’t created by revolution or extrusion.
Just one important note - to use extruded or revolved mesh in PrePoMax, partitions made in CAD software can’t be done in such a way that multiple parts are created from the imported STEP file, and compounding is required (those meshing algorithms don’t support compound parts, and it would be necessary to use tie constraints or merge the nodes). In fact, it’s sufficient to split only the source face (the one selected for the extrusion/revolution). Selection by angle helps with that.
Also, revolution is not applicable to parts spanning 360 degrees (in fact, it even fails for my FreeCAD model of a tube when it’s revolved with some angles well above 300 degrees), but it’s advised to use symmetry anyway, so it shouldn’t be a problem.
However, let’s keep in mind that the OP’s design has non-rotational features.
