Contact Analysis (Part 2)
Contact Analysis (Part 2)
This analysis uses the data of tutorial/10_contact_2tubes
.
Analysis target
The analysis is a cylindrical indentation problem, and the geometry of the analysis target is shown in Figure 4.10.1 and the mesh data is shown in Figure 4.10.2.
Item | Description | Notes | Reference |
---|---|---|---|
Type of analysis | Non-linear static analysis(elastic,contact) | !SOLUTION,TYPE=NLSTATIC !CONTACT | |
Number of nodes | 4,000 | ||
Number of elements | 2,888 | ||
Element type | Eight node hexahedral element | !ELEMENT,TYPE=361 | |
Material name | M1 | !MATERIAL,NAME=M1 | |
Material property | ELASTIC | !ELASTIC | |
Boundary conditions | Restraint,Forced displacement | ||
Matrix solution | Direct method | !!SOLVER,METHOD=MUMPS |
Fig. 4.10.1: Shape of the analysis target
Fig. 4.10.2: Mesh data of the analysis target
Analysis content
The Lagrangian multiplier method is used to perform contact analysis to give the forced displacement in the push-in direction to the forced surface shown in Figure 4.10.1. The analytical control data is shown below.
Analysis control data 2tubes.cnt
.
# Control File for FISTR
## Analysis Control
!VERSION
3
!SOLUTION, TYPE=NLSTATIC
!WRITE,RESULT
!WRITE,VISUAL
## Solver Control
### Boundary Conditon
!BOUNDARY, GRPID=1
X0, 1, 3, 0.0
Y0, 2, 2, 0.0
Z0, 3, 3, 0.0
!BOUNDARY, GRPID=2
X1, 1, 1, 0.0
!BOUNDARY, GRPID=3
X1, 1, 1, -1.0
!CONTACT_ALGO, TYPE=SLAGRANGE
!CONTACT, GRPID=1, INTERACTION=FSLID, NPENALTY=1.0e+2
CP1, 0.0, 1.0e+5
### STEP
!STEP, SUBSTEPS=4, CONVERG=1.0e-5
BOUNDARY, 1
BOUNDARY, 3
CONTACT, 1
### Material
!MATERIAL, NAME=M1
!ELASTIC
2.1e+5, 0.3
### Solver Setting
!SOLVER,METHOD=MUMPS
## Post Control
!VISUAL,metod=PSR
!surface_num=1
!surface 1
!output_type=VTK
!END
Analysis procedure
Execute the FrontISTR execution command fistr1
.
$ cd FrontISTR/tutorial/10_contact_2tubes
$ fistr1 -t 4
(Runs in 4 threads.)
Analysis results
The results of the fourth substep are shown in Figure 4.10.3. A deformation diagram with Mises stress contours is created by REVOCAP_PrePost. A part of the analysis results log file is shown below as numerical data for the analysis results.
Fig. 4.10.3: Analysis results of deformation and Mises stress
Analysis results log 0.log
.
fstr_setup: OK
#### Result step= 0
##### Local Summary @Node :Max/IdMax/Min/IdMin####
//U1 0.0000E+00 1 0.0000E+00 1
//U2 0.0000E+00 1 0.0000E+00 1
//U3 0.0000E+00 1 0.0000E+00 1
//E11 0.0000E+00 1 0.0000E+00 1
//E22 0.0000E+00 1 0.0000E+00 1
//E33 0.0000E+00 1 0.0000E+00 1
//E12 0.0000E+00 1 0.0000E+00 1
//E23 0.0000E+00 1 0.0000E+00 1
//E31 0.0000E+00 1 0.0000E+00 1
//S11 0.0000E+00 1 0.0000E+00 1
//S22 0.0000E+00 1 0.0000E+00 1
//S33 0.0000E+00 1 0.0000E+00 1
//S12 0.0000E+00 1 0.0000E+00 1
//S23 0.0000E+00 1 0.0000E+00 1
//S31 0.0000E+00 1 0.0000E+00 1
//SMS 0.0000E+00 1 0.0000E+00 1
##### Local Summary @Element :Max/IdMax/Min/IdMin####
//E11 0.0000E+00 1 0.0000E+00 1
//E22 0.0000E+00 1 0.0000E+00 1