Fill out the form to download

Required field
Required field
Not a valid email address
Required field
Required field
  • Set up your own cloud-native simulation in minutes.

  • Documentation

    Validation Case: Thick Plate Under Pressure

    This validation case belongs to pressure load in solid mechanics. The aim of this test case is to validate the following parameters:

    • Distributed pressure
    • Nodal stress

    The simulation results of SimScale were compared to the numerical results presented in [NAFEMS]\(^1\).


    The geometry used for the case is as follows:

    geometrical model of thick plate under pressure
    Figure 1: Geometry model for the thick plate

    The plate has a thickness of 0.6 \(m\). Table 1 presents the coordinates for each point:

    PointX [\(m\)]Y [\(m\)]Z [\(m\)]
    D2 00.6
    Table 1: Coordinates of the geometry points

    The point B” is located at the middle of edge BB’ while point C” is located at the middle of edge CC’. The curves of edges BC and AD are defined by equations 1 and 2 respectively:

    $$ ( \frac{x}{3.25} )^2 + ( \frac{y}{2.75} )^2 = 1 \tag{1} $$

    $$ ( \frac{x}{2} )^2 + y^2 = 1 \tag{2} $$

    Analysis Type and Mesh

    Tool Type: Code_Aster

    Analysis Type: Static Linear

    Mesh and Element Types:

    All meshes were computed locally and uploaded to the platform. Table 2 presents the details of the meshes used for each case:

    CaseMesh TypeNumber of
    Element Type
    A1st Order Tetrahedral26639Standard
    B2nd Order Tetrahedral194237Standard
    C1st Order Hexahedral36Standard
    D2nd Order Hexahedral111Standard
    E1st Order Hexahedral105Standard
    F2nd Order Hexahedral349Standard
    G2nd Order Hexahedral52941Standard
    Table 2: Number of mesh nodes and types of elements for each case
    tetrahedral mesh of thick plate under pressure
    Figure 2: Tetrahedral mesh employed for Case B
    hexahedral mesh of thick plate under pressure
    Figure 3: Hexahedral mesh employed for Case G

    Simulation Setup


    • Linear Elastic Isotropic:
      • \( E = \) 210 \( GPa \)
      • \( \nu = \) 0.3

    Boundary Conditions:

    • Constraints:
      • Face DCD’C’ with zero y-displacement
      • Face ABA’B’ with zero x-displacement
      • Face BCB’C’ with zero y- and x-displacements
      • Edge B”C” with zero z-displacement
    • Loads:
      • Pressure of 1 \(MPa\) applied on face ABCD

    Reference Solution

    The reference solution as presented in [NAFEMS]\(^1\) is of the numerical type. For the comparison purposes, the normal stress at point D in the direction of the Y axis is taken:

    \( \sigma_{ref} = 5.38\ MPa \)

    Result Comparison

    Comparison of stress \(\sigma_{yy}\) magnitude computed at the location of point D (variable SIYY) from the simulation results is presented with respect to the reference solution \(\sigma_{ref}\):

    CASE\( \sigma_{ref} \)
    \( \sigma_{YY} \)
    A5.385.16166-4.06 %
    B5.385.400750.39 %
    C5.383.98345-25.96 %
    D5.385.470911.69 %
    E5.385.10811-5.05 %
    F5.385.710586.14 %
    G5.385.385990.11 %
    Table 3: Point D stress results comparison

    The von Mises stress color plot is presented for the results of case G:

    von mises stress color plot of thick plate under pressure
    Figure 4: Von Mises stress result contours from case G


    • (1987) ”The Standard NAFEMS Benchmarks”, “The international association for the engineering analysis community”


    If you still encounter problems validating you simulation, then please post the issue on our forum or contact us.

    Last updated: September 4th, 2023