but this is not applicable to plane stress/plane strain elements, only to shells.
there is a previous post on the subject, basically âyou do not need to look at it, take it as zero (even if value reported is wrong)â. Calculations are right.
I mean the opposite - the quote says that the edge load in force per unit length is only available for shells so it canât be available for plane stress elements and thus only regular pressure in force per unit surface is used for them.
Yes, the total force F is different but A in sigma=F/A is different too. However, there are other effects and results (like a reaction force) that will differ.
right, I misunderstood you. My apologies.
Iâm lost.
Plain Stress, shell loaded on a single side and supported on the other. No matter if load is applied as Line load on the edge or itâs equivalent Pressure over the edge surface, once the value has been set up, result should be thickness independent.
Double thickness, Double edge surface ; 10 thickness, 10 surface. Both , Reaction force and Surface increase in the same proportion as P is fixed.
Stress should be the same.
Could you share the inp file.? Or at least ,square dimensions,hole diameter and material properties.?
If not I could use mine but we couldnât compare with ansys
Yes, thatâs what I meant in my previous post. I just added that some other results like a reaction force will change.
2D Plane Stress:
I have set up the shells as orthotropic to make them closer to plain stress.
*MATERIAL,NAME=1000mm
*ELASTIC,TYPE=ENGINEERINGCONSTANTS
210000000000,210000000000,210000000000,0.3,0,0,80769000000,0
0
*DENSITY
7850
*MATERIAL,NAME=1mm
*ELASTIC,TYPE=ENGINEERINGCONSTANTS
210000000000,210000000000,210000000000,0.3,0,0,80769000000,0
0
*DENSITY
7850
*SOLID SECTION,ELSET=Default,MATERIAL=1000mm
1
*SOLID SECTION,ELSET=Component,MATERIAL=1mm
0.001
CPS4/CPS4R Traction and Pressure: The shell behaves with nice results with Plain Stress behavior:
Szz and z=0
Syz=0
Szx=0
Expected Principal Stress=166.6 MPa
Result Principal Stress= 164.1-167.8 MPA
Thickness independent.
CPS8/CPS8R Traction The shell behaves with nice results and with Plain Stress behavior:
Szz and z=0
Syz=0
Szx=0
Thickness independent.
CPS8/CPS8R Pressure : Wrong result. Displacements explode in z direction .
Sz and z>>>0
Syz=0
Szx=0
PICTURE: CPS8. TRACTION LOADED.Thickness independence.
Nice finding to take into consideration. 
Providing a residual (but not zero) out of plane Shear Modulus G13 and G23 with their corresponding
Poissonâs ratios nu13 and nu23 avoids second order elements to explode when pressure is applied and with good agreement with the theory and Plane Stress expected behavior. (That is to say , Szz, Sxz and SyZ close to zero).
*MATERIAL,NAME=M1000mm
*ELASTIC,TYPE=ENGINEERINGCONSTANTS
210000000000,210000000000,210000000000,0.3,0.000001,0.000001,80769000000,0.0001
0.0001
*DENSITY
7850
*MATERIAL,NAME=M1mm
*ELASTIC,TYPE=ENGINEERINGCONSTANTS
210000000000,210000000000,210000000000,0.3,0.000001,0.000001,80769000000,0.0001
0.0001
*DENSITY
7850
*SOLID SECTION,ELSET=1000mm,MATERIAL=M1000mm
1
*SOLID SECTION,ELSET=1mm,MATERIAL=M1mm
0.001
it seems discrepancy in stress output results of Mises stress due to Szz exist in expanded element. However, when result compared to 3d model of solid element with and without restrained out of plane displacement at support shown still reliable. Below my simple example (left edge fixed and uniform load at top), CalculiX plane stress element result is similar to unrestrained conditions.
Dx,Dy (fixed)
Dx,Dy,Dz (fixed)
Dx,Dy (fixed)
I donât agree.
Here another example with same loading configuration but different thicknesses. (Expanded view of CPS4 elements)
CPS4 elements, 1mm and 1000mm one on top of the other for comparison.
Upper set of Pictures considers CPS4 where Szz, Syz and Sxz are minimized by means of the workaround explained above.
Lower set of Pictures considers CPS4 but with a regular Elastic material definition.
Plain Stress compliant is thickness independent while bottom is not.
VM results deviates considerably.
Bottom could be âcomparableâ to the z-unrestrained 3D solid element but isnât âreliableâ as a Plane Stress Solution.
the same problem as previously but using plane strain element instead, assumption thickness in perpendicular direction are multiple times its sectional dimensions.
p.s try doing comparison with 3d solid element whenever possible, is degenerates element such as 2D or 1D of classical element reliable enough or not. Probably all of them will underestimate in results since the stress actually not zero as plane stress assumptions.
only for matching purpose: use linear quadrilateral with reduced integration (CPS4R) and limit the thickness to about 1/10 sectional dimensions. Material provide as is without any modifications or such a tricky.
So, you are suggesting:
1-
Letâs say limiting the user inputs and available elements to one.
2-
Letâs say computing twice the same model to see if that approach fits what one would normally do but doesnât because is too expensive computationally.
Why not reconsidering the material definition to recover the expected behavior and match a leader comercial solvers?
Are there any negative aspects that I am overlooking about using an orthotropic material?. ÂżMaybe computationally?
I donât see that as a trick. Maybe more like reconsidering if ISO material was the right way to define a Plain Stress expanded shell.
Not really. Tested at least 10 different load configurations and all of them showed higher VM value for the shell when Szz=0 (Plain Stress Compliant).