The setup you have created would not qualify for using the "Inertial Relief" option. That option requires that you have applied equal and opposite forces to the model such that the net force balances out to zero (SOLIDWORKS Help - Simulation: Inertial Relief). The pressure applied to the model is significantly non-zero in the -Z direction though. So, first thing to do is turn that option off.
Once you have that option off you need to think about how to stabilize the model in a way that does not adversely impact the results. Looking at your loading and the shape of the model this can readily be done by cutting out a corner of the model and applying 'Symmetry' fixtures to the resulting cut faces (GoEngineer - SOLIDWORKS Simulation: Symmetry Constraints). This would take care of stability for all rigid body translations/rotations except for the Z-direction translation.
Since you noted that this object is going to be set on a surface you would want to restrain the model by placing a 'Virtual Wall' contact condition for the model to push against (SOLIDWORKS Help - Simulation: Virtual Wall Contact). This stabilizes the Z-direction and lets the model then solve to completion.
It does look like you end up with a stress concentration (possibly a singularity) after 5 iterations of h-adaptive mesh. You may want to modify the geometry of the model in this place to have a fillet to help alleviate this as perfect sharp corners are not common for inside corners in manufacturing.
Attached is a modified model showing the setup itself.
Thanks for the model. I've used it for some simulations and it's working out nicely.
Initially there wasn't any fillet, and my results have been giving me a stress hotspot at that particular location.
I've added a fillet (2mm) on it after that (https://imgur.com/a/tzr1K ) and the same max stress was located there.
I'd like to ask if this is a stress singularity: https://imgur.com/a/hnzxm
I'm curious if such a thing can happen in areas where fillet is present.
That area has been the area of max stress every single iteration of simulation.
Here're some results I've tried to do to determine mesh convergence:
Mesh size --- Max displacement \\ Max stress
3mm ------- 7.678e-2 \\ 1.266e8
4mm ------- 7.673e-2 \\ 1.244e8
8mm ------- 7.647e-2 \\ 1.106e8
16mm ------- 7.575e-2 \\ 1.184e8
32mm ------- 7.405e-2 \\ 0.934e8
64mm ------- 7.159e-2 \\ 0.854e8
128mm ------- 6.938e-2 \\ 0.747e8
256mm ------- 6.302e-2 \\ 0.570e8
512mm ------- 5.099e-2 \\ 0.509e8
** Aside from that, I'd also like to ask if I can use the max displacement trend to determine a mesh convergence point that I will then use to determine the max stress?
Thank you so much
Fillets can help negate stress singularities but they are not a golden bullet for negating them. I am curious about one part of your description though. You have applied a 2mm fillet but the smallest mesh element size you have tested i still larger than that (3mm). Have you yet applied a mesh control to the fillet that goes smaller than 2mm? Are the mesh size values you list above the general mesh size or do these refer to mesh controls values?
The mesh values listed are general mesh size - I did not add mesh controls at all.
After reading your reply, I've tried including a mesh control of 1mm, with a/b ratio of 1.5, to the fillet and re-ran the simulation, with general mesh size at 4mm.
The results actually showed an even higher increase in max stress (1.8 e8 now), as compared to when I did not add the mesh control (1.2e8).
I'm now thoroughly confused as to what the issue is here.
All indications point to this being a stress singularity but you will probably just want to try one more run with the mesh control set to 0.5mm and see if the stress commensurately skyrockets.
I've redone the simulation with 0.5 mesh control (same a/b ratio)
The resulting max stress was 1.893e8, same area. (0.030e8 increase vs 1mm control)
It looks like you are about converged then. You have made a large change to the size of mesh elements in that region of the model (50% reduction) and it changed only a minor amount of the stress value (less than 2% increase in stress). In the end, you're the analyst though. Just make sure you are satisfied with the result.
A few things:
- Your model will never be in equilibrium as a pressure vessel because there are holes/voids in the wall. Somewhere in the system there has to be containment. I have in the past put a reaction at the openings equal to P x Area of the opening.
- When you have the pressure balanced you can use a "soft spring" (not inertial relief) to tell the solver that this thing shouldn't move.
- Generally, local stress hot spots will occur in an analysis of this type. No amount of filleting or mesh refinement will remedy this. You may want to look at the stress linearization feature of Simulation which assists in "smoothing out" results.
- I highly recommend using surfaces/shells for this work at it is more efficient and, properly restrained, more accurate.
Let me know if you have any questions.
Thanks for the reply. I've tried using symmetry and virtual wall contact as per Ryan's advice (see above). Stabilising doesn't seem to be an issue now.
I've briefly read through the linearization feature. Apparently it works with pressure vessel study instead of static study? I've no knowledge of how to proceed with a pressure vessel study (even though my work is on pressure vessels...).
Regarding surfaces/shells, is it possible if I can have a detailed explanation as to what I should do and what it does?