9 Replies Latest reply on Feb 5, 2018 11:11 AM by Ryan Dark

    Need help with simulation (constraints etc.)

    Eddie Chua

      Hi all, I'm currently doing a project and am tasked to design a rectangular chamber to withstand certain vacuum and/or positive pressure.


      I've come up with the design. However now the issue is with simulations that I should be doing on the chamber.


      Are there any rules or steps to ensure an accurate simulation?


      I've been running a few iterations (following some steps I found online) and I'm not sure if I can trust the results. Though I'm rather certain it shouldn't fail since the pressure involved is low, but I'd like to have some accuracy to show for my report.


      So generally, I would select a Static Study (I've seen some comments on doing a buckling study, but I've yet to look into it).


      Then apply pressure on the inside/outer walls of the chamber (1bar vacuum or 3bar pressurised).


      What I'd like to ask is:


      1) Restraints. If my chamber is to be rested on a frame (not nailed or bolted), how do I restraint it? I've seen some comments suggesting Inertial Relief, but some other comments say it gives quite some error.


      2) Mesh. I selected Standard mesh at 5mm. I understand I need to do mesh independence/convergence tests, but the max stress still trends upward while my computational power starts to suffer. Can't seem to reach a convergence point. I've seen suggestions to do H-adaptive studies. Is that a possible solution? Also, how would I know if the adaptive study reaches the percentage accuracy by the fifth iteration?


      I've attached a picture of the chamber without its cover below.



        • Re: Need help with simulation (constraints etc.)
          Ryan Dark

          Hi Eddie,

          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.

            • Re: Need help with simulation (constraints etc.)
              Eddie Chua



              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

            • Re: Need help with simulation (constraints etc.)
              Attilio Colangelo

              Hi Eddie,


              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.



                • Re: Need help with simulation (constraints etc.)
                  Eddie Chua



                  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?


                  Thank you.