Hi!
I haved a lot of problems trying to simulate a pipe indentation using *CONTACT. In this problem a spherical body must indents (in radial direction) a pipe. A displacement BC is used to move the spherical body against the pipe. I’m using 8-node hexahedral elements along with *CONTACT PAIR, INTERACTION=CONTACT,TYPE=NODE TO SURFACE and *SURFACE BEHAVIOR, PRESSURE-OVERCLOSURE=EXPONENTIAL. However, no convergence was possible!
Link to input file (*.inp):
Thanks in advance!
Jack
i took ur .inp file and opened it in Mecway and some of the units were rather odd - very low E and the ball was being moved 6 m! I changed to what looked like more sensible units and ran a quasistatic non linear analysis and used a simple conatct and it all appeared to work ok
I used a node/surface coupling to move the ball rather than move the entire surface - most of the .inp was the same as yours -the different parts were as below
*RIGID BODY,NSET=node-surface_coupling_faces,REF NODE=23970,ROT NODE=23971
*AMPLITUDE,NAME=A_1
0,0
1,-0.007
*CONTACT PAIR,INTERACTION=SI_2,TYPE=SURFACE TO SURFACE
contact_faces(2),contact_faces
*SURFACE INTERACTION,NAME=SI_2
*SURFACE BEHAVIOR,PRESSURE-OVERCLOSURE=LINEAR
3000000000000
*STEP
*STATIC,TIMERESET,SOLVER=PARDISO
*EL FILE
ENER
*END STEP
*STEP,NLGEOM=YES,INC=100,AMPLITUDE=STEP
*STATIC,SOLVER=PARDISO
0.01,1,0,0.05
*BOUNDARY,AMPLITUDE=A_1
23970,2,1
*DSLOAD
DLOAD_faces,P,1
*NODE FILE,GLOBAL=YES
U,RF
*EL FILE
S,NOE,E,ENER
*NODE PRINT,GLOBAL=YES,NSET=ref_and_rot_nodes
RF
*END STEP
Thank you so much. Now is working!
However, I see C3D8 elements too stiff for this problem. C3D8I or C3D20 elements would work better? Or may be C3D4 o C3D6 instead?
Thanks in advance,
Jack.
Different element types are nicely summarized in the documentation:
C3D8:
Although the structure of the element is straightforward, it should not be used in the following situations:
- due to the full integration, the element will behave badly for isochoric material behavior, i.e. for high values of Poisson’s coefficient or plastic behavior.
- the element tends to be too stiff in bending, e.g. for slender beams or thin plates under bending.
C3D8I:
The C3D8I element should be used in all instances, in which linear elements are subject to bending. Although the quality of the C3D8I element is far better than the C3D8 element, the best results are usually obtained with quadratic elements (C3D20 and C3D20R). The C3D8I element is not very good when subjected to torsion.
C3D8R:
Due to the reduced integration, the locking phenomena observed in the C3D8 element do not show. However, the element exhibits other shortcomings:
- The element tends to be not stiff enough in bending.
- Stresses, strains… are most accurate in the integration points. The integration point of the C3D8R element is located in the middle of the element. Thus, small elements are required to capture a stress concentration at the boundary of a structure.
- There are 12 spurious zero energy modes leading to massive hourglassing: this means that the correct solution is superposed by arbitrarily large displacements corresponding to the zero energy modes. Thus, the displacements are completely wrong. Since the zero energy modes do no lead to any stresses, the stress field is still correct. In practice, the C3D8R element is not very useful without hourglass control. Starting with version 2.3 hourglass control is automatically activated for this element, thus alleviating this issue.
C3D20:
This is an excellent element for linear elastic calculations. Due to the location of the integration points, stress concentrations at the surface of a structure are well captured. However, for nonlinear calculations the elements exhibits the same disadvantages as the C3D8 element, albeit to a much lesser extent:
- due to the full integration, the element will behave badly for isochoric material behavior, i.e. for high values of Poisson’s coefficient or plastic behavior.
- the element tends to be too stiff in bending, e.g. for slender beams or thin plates under bending.
C3D20R:
The element behaves very well and is an excellent general purpose element (if you are setting off for a long journey and you are allowed to take only one element type with you, that’s the one to take). It also performs well for isochoric material behavior and in bending and rarely exhibits hourglassing despite the reduced integration (hourglassing generally occurs when not enough integration points are used for numerical integration and spurious modes pop up resulting in crazy displacement fields but correct stress fields). The reduced integration points are so-called superconvergent points of the element. Just two caveats:
- the integration points are about one quarter of the typical element size away from the boundary of the element, and the extrapolation of integration point values to the nodes is trilinear. Thus, high stress concentrations at the surface of a structure might not be captured if the mesh is to coarse.
- all quadratic elements cause problems in contact calculations, because the nodal forces in the vertex nodes equivalent to constant pressure on an element side (section ) are zero or have the opposite sign of those in the midside nodes. This problem seems to be solved if face-to-face penalty or mortar contact is used.
C3D4:
This element is included for completeness, however, it is not suited for structural calculations unless a lot of them are used (the element is too stiff). Please use the 10-node tetrahedral element instead.
C3D10:
The element behaves very well and is a good general purpose element, although the C3D20R element yields still better results for the same number of degrees of freedom. The C3D10 element is especially attractive because of the existence of fully automatic tetrahedral meshers.
C3D6:
This element is included for completeness, however, it is probably not very well suited for structural calculations unless a lot of them are used. Please use the 15-node wedge element instead.
C3D15:
The element behaves very well and is a good general purpose element, although the C3D20R element yields still better results for the same number of degrees of freedom. The wedge element is often used as fill element in "automatic’’ hexahedral meshers.
So basically, use C3D8I / C3D8R or C3D20 / C3D20R if the geometry allows that. The exact choice depends on the case (bending, stress concentrations, hyperelasticity/large plastic strains, …).
Now is working! Thanks a lot.
Now I trying to run the same problem but now using shell elements (S4) in the pipe. However, convergence problems appears when plastic deformation rises. Model doesn’t converge for plastic strains beyond to yield stress. This is the link to *.inp of the model:
Thanks in advance.
Jack
This input file is incorrect, it causes various syntax errors - at least with *TIME POINTS and *SURFACE (missing elset “Suptubo”).
Sorry, here *.inp fixed:
Tanks,
Jack
