Validation Case: 3D Triaxial Displacement Secondary Creep (NAFEMS Test 6(b))

The secondary creep validation case belongs to solid mechanics. This test case aims to validate the following parameters:

Creep material behavior
Standard and reduced integration elements
Automatic time stepping

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

View Project

Geometry

The geometry consists of a cube with an edge length \(l\) = 0.1 \(m\).

The coordinates for the points in the cube geometry are as tabulated below:

	A	B	C	D	E	F	G	H
x	0	0.1	0.1	0	0	0.1	0	0.1
y	0	0	0.1	0.1	0	0	0.1	0.1
z	0	0	0	0	0.1	0.1	0.1	0.1

Table 1: Cube dimensions in meters

Analysis Type and Mesh

Tool Type: Code Aster

Analysis Type: Nonlinear static

Mesh and Element Types: The mesh for cases A through D is a second-order tetrahedral mesh, generated in SimScale by the standard algorithm.

Case	Mesh Type	Number of Nodes	Element Type	Creep Formulation	Element Technology
A	Standard	235	2nd order tetrahedral	Norton	Standard
B	Standard	235	2nd order tetrahedral	Norton	Reduced integration
C	Standard	235	2nd order tetrahedral	Time Hardening	Standard
D	Standard	235	2nd order tetrahedral	Time Hardening	Reduced integration

Table 2: Overview of the validation cases. The element technology integration and creep formulation change between the cases.

Find below the standard mesh used for cases A through D:

generated second order mesh in simscale which has 235 nodes for secondary creep validation — Figure 2: Generated second order mesh with SimScale for cases A through D

Simulation Setup

Material:

Steel (linear elastic)
- Isotropic: \(E\) = 200 \(GPa\)
- \(\nu\) = 0.3
- \(\rho\) = 7870 \(kg/m³\)
- Creep formulation:
  - Time hardening
    - A: 8.681e-48 \(1/s\)
    - N: 5
    - M: 0
  - Norton
    - A: 8.681e-48 \(1/s\)
    - N: 5

Boundary Conditions:

Constraints:
- Fixed value:
  - Face ADEH: \(d_x\) = 0 \(m\)
  - Face ABFE: \(d_y\) = 0 \(m\)
  - Face ABCD: \(d_z\) = 0 \(m\)
- Displacement in x-direction
  - Face BCGF: \(d_x\) = 0.3 \(mm\)
- Displacement in y-direction
  - Face CDHG: \(d_y\) = 0.2 \(mm\)
- Displacement in z-direction
  - Face EFGH: \(d_z\) =0.1 \(mm\)

Advanced Automatic Time Stepping

For all cases, the following advanced automatic time stepping settings were defined under Simulation control:

Retiming event: Field change
Target field component: Internal variable V1 (accumulated unelastic strain)
Threshold value: 0.00005
Timestep calculation: Mixed
Field change target: 0.00004

Result Comparison

The secondary creep movement validation is done by comparing the stress (\(\sigma_{xx}\)) after a creep time of 1000 hours. Below you will find the SimScale and reference results from [NAFEMS]\(^1\):

Case	NAFEMS R27 \([MPa]\)	SimScale \([MPa]\)	Error [%]
A	1007.7	1008.23	0.053
B	1007.7	1008.23	0.053
C	1007.7	1008.23	0.053
D	1007.7	1008.23	0.053

Table 3: Stress comparison between the reference and the simulation results

In all configurations, the results obtained with SimScale show a good agreement with the reference values. The displacement of the geometry can be seen below:

visualization of displacement of a cube — Figure 3: Displacement observed in case A

Note

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

Last updated: November 29th, 2023

Did this article solve your issue?

How can we do better?

We appreciate and value your feedback.