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
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

Shape of the analysis target

Fig. 4.10.1: Shape of the analysis target

Mesh data 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.

Analysis results of deformation and Mises stress

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

Contact Analysis (Part 2)