Hello everyone. To start off, I should mention that I am a beginner when it comes to advanced FEM analysis. I have a connection between a timber beam and a reinforced concrete beam using a metal connector, and I want to analyze the connector itself. Could you help me check it and point out any mistakes I might be making? Thanks in advance.
Next time please close the results (File → Close All Results) before saving the file to reduce its size.
You used many volume partitions to get a nicely structured (transfinite) hex mesh. You could just have more elements through the thickness. In fact, it would be easiest to import a surface geometry and use the Thicken Shell Mesh tool to create a hex mesh.
Apart from that, it looks good, assuming that your BCs and load are realistic. I mean mostly things like applying them only to one side of the hole. Perhaps you could use compression-only constraint for them or even bearing load-like pressure distribution.
1 Like
Here’s what I mean with Thicken Shell Mesh to have more element layers through the thickness:
Łącznik dźwigara - kątownik z powierzchni.pmx (5.4 MB)
Just pay attention to mesh quality - elements shouldn’t be too stretched and you may need to adjust the partitions to get better shapes or use a different algorithm than Quasi-structured quad.
1 Like
Thank you. I tried using a compression-only constraint to apply the load, but I couldn’t get the model to converge. I also wanted to use a compression-only constraint on the horizontal arm instead of a rigid support, but I ran into major convergence issues there as well. I lacked the knowledge to resolve this.
To use compression-only constraint to apply load, you would have to sort of invert the loading scheme (pull from the other side):
Or you could edit keywords, connect the end nodes of GAP elements with rigid body constraint and apply load through them: Multibody parts connection - #4 by FEAnalyst
1 Like
Regarding convergence with compression-only constraints, reducing the stiffness (a lot) and increasing the tensile force usually helps. Unless it wouldn’t converge anyway just because of introducing nonlinearity.
1 Like
I made changes to the model and applied “compression-only” settings to the bolt holes in the vertical and horizontal arms of the angle bracket—and once again, there is no convergence.
Please don’t use the code tags (```) for regular text, it’s hard to read.
Your compression-only constraints used for the holes still have large spring stiffness and default tensile force:
Did you try decreasing the stiffness (by several orders of magnitude) and increasing the tensile force (at least to 0.1 N or 1 N) ?
You can also try replacing Nlgeom with dummy nonlinearity introduced by the Nonlinear option in compression-only constraint settings.
1 Like
Thank you so very much. For the help and the tip. Everything is working now 
When it converges, you can always try increasing these values back (especially tensile force) to see how much you need to reduce them to achieve convergence. You can also try restoring Nlgeom if needed. Just notice that I’ve changed some incrementation settings too. And I would use a different mesh, as explained yesterday.
Okay. Thanks again for your help. I’ll try creating a model from surfaces and experimenting with the settings.
Sure, I attached an example here: Reinforced carpentry angle bracket - #3 by FEAnalyst
It was prepared in FreeCAD based on your solid geometry exported to step format. Let me know if you need more information about this workflow involving FreeCAD.
I’m not familiar with FreeCAD at all, so I tried creating the surface in AutoCAD, but unfortunately, I didn’t succeed. The IGES file loads into PrePoMax, but when I generate the FEM mesh, everything disappears and the screen goes blank
Indeed, the Thicken Shell Mesh tool fails for this surface geometry. If you share your original solid model again, I can show you how to do it in FreeCAD step by step.
@Matej If I use the Thicken Shell Mesh tool in the FE Model tab, it looks like this:
Thicken Shell Mesh bug.pmx (730.7 KB)
I’ve tried it in v2.6.0.
Ok, here are the steps to do it in FreeCAD:
- Export the compound from PrePoMax (select it and use File → Export → Step).
- Import it to FreeCAD (File → Import).
- Switch to the Draft workbench, select all faces on one side of the bracket and use the Facebinder tool:
- Switch to the Part workbench, select the Facebinder in the model tree and activate the 3D Offset tool:
- Enter -1.5 as offset value. You will get a midsurface of the bracket:
- Export the Offset object to .step file and import it to PrePoMax.
1 Like
The problem are the face orientations.
Fixing them creates a valid mesh.
I will add a surface orientation check.
All right, good to know. I thought it only mattered for thickening with offset.