LE10: Thick plate under pressure

The Abaqus/Standard results are shown in Table 1. The values enclosed in parentheses are percentage differences with respect to the reference solution.

Table 1. Abaqus/Standard analysis.

Element	${\sigma }_{yy}$, Coarse Mesh	${\sigma }_{yy}$, Fine Mesh
C3D20	−6.72 MPa (+25.00%)	−5.64 MPa (+4.83%)
C3D20R	−7.93 MPa (+47.39%)	−5.53 MPa (+2.78%)
C3D10	−5.44 MPa (+1.15%)	−5.77 MPa (+7.24%)
C3D10HS	–5.08 MPa (−3.72%)	–5.51 MPa (+2.42%)
C3D10M	−5.57 MPa (+3.53%)	−5.89 MPa (+9.48%)

The C3D10 and C3D10M elements are more accurate with the coarse mesh than with the fine mesh: in the coarse meshes four elements come together at the point of interest, giving a more accurate result after averaging to the nodes. In the more refined mesh, only one element contains the point of interest; therefore, the extrapolation to the nodes is less accurate.

Unlike Abaqus/Standard, Abaqus/Explicit does not have the option for extrapolating integration point outputs (such as stresses) to the nodes. Consequently, the desired stress component at point D cannot be extracted except by rough interpretation of color contour plots. As an alternative, the value of ${\sigma }_{yy}$ at an integration point near point D is compared between an Abaqus/Standard simulation and an Abaqus/Explicit simulation.

In the Abaqus/Explicit analyses the pressure is ramped up smoothly from zero to its final value of 1.0 MPa over a time period of 0.4 seconds, which is slow enough to be considered quasi-static (inertial effects play a minimal role).

Analysis Type	${\sigma }_{yy}$, Coarse Mesh	${\sigma }_{yy}$, Fine Mesh
Abaqus/Standard	−3.70 MPa	−4.61 MPa
Abaqus/Explicit	−3.79 MPa	−4.55 MPa

For the coarse mesh the point of comparison is at element 18, integration point 3. For the fine mesh the point of comparison is at element 199, integration point 1. Both are close neighbors of the physical corner point D.