Always use quad elements for shells.
For parameters, see the attachment.
Meshing depends on the geometry.
shell.pmx (609.4 KB)
Link: WeTransfer - Send Large Files & Share Photos Online - Up to 2GB Free
shell.pmx (609.4 KB)
I could not open shell.pmx.
Here is another problem. I put a load on the file Saturday4.pmx and the part with the load separated from the rest. Can you merge loads in PrepoMax like you could in ANSYS?
Thank you.
https://drive.google.com/drive/folders/1E3xuipgce2e53yVlFEPl1RGQdyfNK64b?usp=sharing
You have to connect the parts. Either by creating a compound part or with tie constraints. To check the connections, use a Frequency analysis - you will see the parts flying away.
Apart from that, the mesh is too coarse, there’s still a concentrated force load on the surface while boundary condition is strangely applied only to the edges.
I have made the problem as simple as I can. It is just the pipe from the vessel and the flange.
I anchored the bottom and put a load on top. This should be basically a cantilever beam. As you can see the flange separates from the pipe. In other programs I would select the nodes between them and say merge nodes.
What is wrong here?
Thank you.
https://drive.google.com/drive/folders/1E3xuipgce2e53yVlFEPl1RGQdyfNK64b?usp=sharing
Just apply a tie constraint between the two parts (it can even be defined automatically with the Search Contact Pairs tool).
Thank you for your help.
I need to study the difference between compound part, merge and rigid connection.
Thank you.
They are described in the manual. The Merge option only assigns elements from multiple parts to one part without changing the mesh so it won’t connect the parts. For that, you need the Compound part tool. Sometimes it fails due to inaccuracies in alignment or when the parts are STL (it’s meant for CAD parts). Then you can use tie constraint to connect the nodes during the analysis.
Meshing parameters see pictures.
Regarding the last issue, see the attachment.
saturday6_nozzle and flange.pmx (7.6 MB)
I hope it is useful.?
I’m using PrePoMax 2.1.2.
Here is a model with some results but I don’t believe them.
The high stresses are in a small concentrated area.
The nodes do not seem to line up between the vessel dome and the nozzle.
https://drive.google.com/drive/folders/1E3xuipgce2e53yVlFEPl1RGQdyfNK64b?usp=drive_link
That’s normal when using tie constraints. They don’t need matching meshes. But you should refine the meshes properly and keep in mind that the master surface should have a coarser mesh. Then you can use Adjust and Position tolerance settings to ensure proper connection. Still, stresses directly where tie constraints are located may not be realistic. Merging meshes is better but sometimes fails. Here you could also consider using shell model (on surface geometry). Then the connection would also be simplified but you would get better global results (now you have just one tetrahedron in the thickness direction everywhere). You could even use solids for the connection region and tie them to shells in the remaining part of the model. Then add some fillet for more realistic results.
1 Like
As FEAnalyst noted, this can be a hot spot (singularity) due to boundary conditions (tie) and also mesh. My suggestion: use only one part, make an appropriate mesh (preferably Hex) and refine it after checking.
P.S.: because the geometry is not clean, export the geometry as *.stp, correct it in the CAD program and import it again (sometimes it is enough to just export and then import the geometry).
When you say use one part, does that mean making a compound part?
Thank you.
George
It’s best to make one part in CAD, otherwise make a compound part.
1 Like