This element can be used to control the contact between one node and a face. The face is a triangular or a quadrangular facet in a 3-D analysis or a segment in 2-D analysis.
The node candidate to contact is first defined. Afterwards, the nodes belonging to the face are defined according to the logic used in the .MAI command.
For a triangular facet, the positive normal is defined by the cross product of the side N2-N3 by the side N2-N4, if N2 N3 N4 are the corner nodes of the face. For a quadrangular facet, the positive normal is defined by the cross product of the side N2-N4 by the side N3-N5, if N2 N3 N4 N5 are the corner nodes of the face. For a segment, the positive normal is defined by the cross product of the Z vector by the side N2-N3, if N2 N3 are the corner nodes of the 2-D face. The normal to the facet points to the allowed region for slave nodes.
Friction forces can be taken into account. It is possible to introduce a deformable contact (law between the contact pressure and the clearance). It is also possible, in a dynamic analysis, to introduce some viscous damping.
Usually, the contact elements are defined with the .MCT macro-command using as input a group of nodes and a group of faces or elements. In this case, in general, the surface linked to the node candidate to contact will be computed.
The element has a variable number of degrees of freedom, depending on the definition of the face, distributed as follows:
|Degrees of freedom
|X, Y, Z
|1, 2, 3
|Nodal position vector of the node candidate to contact
|X, Y, Z
|N2, N3, N4, ...
|1, 2, 3
|Nodal position vector of the nodes belonging to the face
|λ1, λ2, λ 3
|7, 8, 9
|3 Lagrange multipliers
|Degree of freedom
|X, Y, Z
|Nodal position vector of the node candidate to contact
|X, Y, Z
|N2, N3, ...
|Nodal position vector of the nodes belonging to the face
|2 Lagrange multipliers
If NLIM in .MCT command is equal to 1 or -1, the Lagrange multipliers are linked to the element. Otherwise they are linked to components 7/8/9 of the slave node.
The contact problem is analyzed in several steps:
computation of the normal distances
contact detection (contact algorithm)
|NLIM EXT UN2 DCON
In the topology search, for each slave node, the software is looking for closest faces. The topology search is made by the .MCT command. It does not depend on the contact algorithm. Different options are possible:
For each node, BACON finds the NLIM closest faces. During the analysis, the node can slide on these NLIM faces. The software has to find if a node/face couple is active or not.
The topology search can be performed at each iteration (default) or only at the beginning of the time step (UN2 2). If it is done only at the beginning of the time step, during the iteration, the faces are extrapolated. This option can reduce the oscillation of the Newton scheme when one node hesitates between two faces. If the topology search is made during the iteration and if NLIM = -1, two options are possible. Either the software takes the closest facet (UN2 0), or if the projection of the node is inside the facet of the previous iteration, taking into account EXT keyword, the facet is not changed (UN2 3). The default value for UN2 is 3 if NLIM = -1 and 0 otherwise. The software has to find if a node/face couple is active or not.
The first test is to compute the distance between the node and the centre of gravity of the face. If this distance is larger than DCON (characteristic length for the contact problem, the way it is defined is described in the remark below), the node/face couple is inactive. The second test is to find the projection of the node on the face. If the intrinsic coordinate of the projection is smaller than (-1-tol) or larger than (1+tol), the node/face couple is inactive. The tolerance "tol" can be defined in an explicit way (EXT -).
The default value of EXT depends on NLIM:
NLIM >1: it is better not to extrapolate the face, default value for EXT is taken equal to 0.01.
NLIM =1: it is better to extend the face, default value for EXT is taken equal to 0.2.
NLIM =-1: it is better to extend the face, default value for EXT is taken equal to 0.05.
NLIM <-1: it is better not to extrapolate the face, default value for EXT is taken equal to 0.01.
The following should be taken into account
In general it is better to use NLIM = -1 or 1. NLIM 1 for small sliding, with an extrapolation of the face. NLIM -1 for large sliding.
In every case (except in linear geometric case), the direction of the normal is updated.
In linear geometric case (ASEF or .SAM NLIS -1), the topology search is never made during the analysis (if NLIM < 0, NLIM is replaced by its absolute value). The test to see if a node/face couple is active or not is made at the beginning of the analysis and does not depend on the displacement.
for ASEF, NLIM must be equal to 1 or -1.
|UN3 DLIM DMIN
The way the normal distance is computed does not depend on the contact algorithm. The purpose is to define when contact appears. By default, contact starts when the normal distance between the node and the face is equal to 0. The normal distance for the contact problem is equal to the physical geometrical normal distance.
|dcontact = dgeometrical
The first option (UN3 1) is to change this 0 value by the initial distance between the node and the face. So as soon as the slave node moves in the direction of the face, contact appears. We will say that the normal distance for the contact problem is equal to the physical geometrical normal distance minus the initial distance:
|dcontact = dgeometrical – dgeometrical_initial
It is useful when there are small imperfections in the nodal coordinates and when the users know that the contact surfaces are close together. This modification is done for the nodes for which the initial distance is smaller than DLIM (default: infinity). It is always done if there is an initial penetration. UN3 1 is equivalent to L 0 in .CPS and .JER commands.
The second option (UN3 2) is to change the 0 value by the initial distance of the node which is the closest of the master surface:
|dcontact = dgeometrical - [dclosest_node]
The same value is applied on all the nodes of the .MCT command. In this way, there is no initial gap between the group of nodes and the group of faces.
The third option, which can be combined with the previous one, is to perform an offset (DMIN) of the face. It can be useful for shell problem (for instance, if the nodes are at the middle surface of the shell, DMIN should be equal the sum of the thickness of the shell divided per 2). It is also useful in order to introduce an initial gap or an initial penetration with or without the first option. The normal distance for the contact problem will be equal to:
|dcontact = dgeometrical – [dgeometrical_initial] - [dclosest_node] - DMIN
For instance, when the user defines the two surfaces in contact at the same place (with some minor mesh imperfection) and wants to introduce a initial penetration (gap), he has to introduce UN3 1 and DMIN initial_penetration (= minus initial gap). UN3 1 DMIN value is equivalent to L-value in .CPS command.
|OPT OPCO CF CFNF
OPT must be equal to 3. The only value allowable for OPCO is 0 (default value). All the data for the topology search and the normal distance computation are available.
The condition on the normal distance is:
|dcontact = dgeometrical – [dgeometrical_initial] - [DMIN] ≤ 0
Without friction, no data are needed for the contact algorithm. With friction, the strategy data are introduced in the .ALG command. The friction coefficient is introduced by CF and can be multiplied by a function of time CFNF.
|OPT OPCO OPFR STIF NPEN UN1 UN4 CF CFNF CFVE CFTE TOL TRTI COMP NDIG
OPT must be equal to 2 (default value).
Different normal behaviors are available:
OPCO 0: standard contact option. The condition on the normal distance is: dcontact ≥ 0 or dcontact = f(pressure)
OPCO 2: bilateral contact option. The condition on the normal distance is: dcontact =0 or dcontact = f(pressure)
OPCO 1: when the contact is closed, it is kept closed, switch from OPCO 0 to OPCO 2 after the first contact.
OPCO 6: no condition on the normal distance, only get the distance in post-processing.
By default, the normal distance is compared to 0. It is possible to introduce a relation between the pressure and the normal distance.
For OPCO 0, the relation can be linear (STIF keyword) or nonlinear (NPEN keyword):
If dcontact < 0: dcontact = pressure/STIF
If dcontact > 0: pressure = 0
NPEN refers to a number of a .FCT function, the interval of definition goes from pmin to pmax.
The abscissa is the pressure; the ordinate is the normal distance.
If pressure < pmin: the curve is extrapolated,
If pmin < pressure < pmax: relation between normal distance and pressure,
If pmax < pressure: not allowed, not in contact, pressure becomes equal to 0.
For OPCO 1, the relation can be linear (STIF keyword) or nonlinear (NPEN keyword):
Linear: dcontact = pressure/STIF
Nonlinear: NPEN refers to a number of a .FCT function, which the interval of definition goes from pmin to pmax. If the pressure is outside the interval of definition, the curve is extrapolated.
When velocity is taken into account (.SUB MECA 1/2/11/12), it is possible to add a contact viscous pressure. The viscous pressure is equal to the product of the velocity of the normal distance and a function of the normal distance. The user has to give as data the number of the .FCT function (keyword UN1).
As tangential behavior, it is possible to take into account friction, to impose shear forces or to couple the shear forces to a control box.
The friction coefficient is introduced by CF and can be multiplied by a function of time CFNF and/or by a function of the relative velocity CFVE (the velocity is computed as the difference of sliding between two time steps divided by the size of the time step) in order to get the transition between static and dynamic friction and/or by a function of the temperature CFTE (function of the mean temperature between slave and master sides). In case of OPFR 1, it is possible to take into account an anisotropic friction behavior. The user has to introduce two values after CF keyword. The friction criteria between stick/slip behavior is an ellipse and the sliding velocity is perpendicular to this ellipse. In case of CFVE, the friction coefficient in the first/second direction depends on the relative velocity in the first/second direction.
Different friction behaviors are available:
OPFR 1: classical friction. By default, the relative displacement is equal to 0 if the friction stress is smaller than the pressure multiplied by the friction coefficient. In order to improve the convergence, it is possible to introduce a stiffness (STFR keyword) between the friction stress and the relative displacement. Once the friction stress becomes equal to the pressure multiplied by the friction coefficient, this stiffness has no more influence. The introduction of the stiffness (STFR keyword) is only available if NLIM = 1/-1. In 3D analysis, if NLIM = -1, a frame must be linked to the element (FRM1 keyword) to allow continuous transitions between elements of the contact boundary condition (.MCT command); the frame should not be defined for 2D contact conditions.
OPFR 2: infinite friction coefficient (CF is not used).
OPFR 3: the friction coefficient depends on the relative velocity (computed in function of the nodal velocity). The friction stress Ffr is directly proportional to the normal reaction between the point and the surface by means of a regularized friction coefficient μR:
|Ffr = μR |Fnorm|
The regularized friction coefficient depends on the relative sliding velocity and takes the form:
where is the relative sliding velocity between the point and the surface, μ is the friction coefficient and εv is a regularization tolerance (TOL keyword) introduced to avoid the singularity of the derivative at = 0 (see below).
When velocity is taken into account (.SUB MECA 1/2/11/12), it is possible to add a contact tangential viscous pressure. The viscous pressure is equal to the product of the tangential sliding velocity and a function of the normal distance. The user has to give as data the number of the .FCT function (keyword UN4).
The shear forces can be introduced in different ways:
OPFR 4: a shear load per unit of surface is applied to the surface of the CONT element. The load can be applied in the 1st (.CLM SFX) and 2nd (.CLM SFY) direction, in element local axis (see FRM1 keyword below). The load is applied to the slave node, and a reaction force is applied to the master face.
OPFR 6: identical to OPFR 4, before a transition time (keyword TRTI, default value 0.00001) a shear load per unit of surface is applied to the surface of the CONT element. It is the same definition as for OPFR 4. After the transition time, the two surfaces are glued. The relative displacement obtained at the end of the last step before the transition time is kept constant for the end of the analysis.
OPFR 7: identical to OPFR 6, except that the user does not introduce a load per unit of surface but the total load applied on all the nodes of the group of the .MCT definition. The total load is divided by the area of the .MCT (slave side). The load (.CLM LFX) can only be applied in the first direction of the element.
The user has to define an attribute in the .MCT command and use this attribute in order to load the element in the .CLM command.
OPFR 5: one can apply the output of a digital controller, that will act as a shear force SFX and/or SFY, as described above.
The controller is defined by:
NDIG -: the element number of the control box,
COMP val1 [ val2]: the components of the COUT vector, of a controller, which acts as loads SFX and SFY respectively.
In order to compute a pressure, the contact force is divided by a surface linked to the node candidate to contact. It is automatically computed by the .MCT command when it is possible to build faces from the nodes of the slave side (otherwise it is put equal to 1). If the user does not use the .MCT command or wants to introduce the surface by himself (for instance if the slave nodes belongs to beams), he has to use keyword DSUR.
By default, the first direction for the tangential behavior is parallel to the first edge of the element. A local frame, defined with the .FRAME command, can be applied to the element. The user refers to the frame number with the FRM1 keyword. The projection of the first axis of the frame on the master face gives the first direction of the element. In non-linear analysis, this direction follows the element.
The automatic time step choice algorithm in dynamic analysis (.SUB IMPL 2 or 22) may be influenced by the necessity of having a time step corresponding to the appearance of contact. To do that, the user can define the maximum variation of the normal distance between the node and the facet during the time step where the contact occurs. If this criterion is not satisfied, the time step is rejected. The maximum variation of normal distance is introduced after DGAP keyword (default value 10-3, absolute value). This keyword has no influence in a static analysis.
1. In the contact problem, there are characteristic lengths which can be introduced at the element level or structural level:
If an automatic time step strategy is used, the maximum variation of displacement along a structural axis during one time step must be smaller than DCON (defined by .SUB). It is defined at the structural level. By default, DCON is equal to 5 times the maximum length of the largest CONT elements.
in the topology search, DCON can be introduced at the element level (.MCT command). By default the structural value is taken.
2. If friction is introduced, it could be useful to use a non symmetrical solver (.SUB command, INLY keyword) if the coupled algorithm is chosen. For the uncoupled algorithm, the non-symmetry of the matrix due to friction is taken into account in the contact problem and it is not useful to use the non symmetrical solver for the friction problem.
3. In MECANO, if the command .SAM NLIS -1 has been introduced, the element is assumed to be linear geometrically. The normal and the projection of the node on the facet are not updated. The topology search is only made at the beginning of the analysis.
4. In order to be compatible with previous SAMCEF version, OPCO 3/4 is automatically translated into OPCO 2/0 and UN3 1.
5. For a MECANO - DYNAM chaining, in case of coupled iterations, if contact is closed in MECANO, it is also closed in DYNAM and, if there is friction, the sliding displacement is fixed in DYNAM. In case of uncoupled iterations, the same behavior is obtained with .ALGO CONFIX
The contour of this element is drawn inside the face of the finite element which supports it.
Provided that their storage has been requested using .SAI ARCHIVE element_selection COMPcomponent_selection, a number of results can be accessed. The table below lists the component numbers available.
|Friction stress (norm)
|Friction stress in the first direction
|Friction stress in the second direction
|Sliding velocity in the first direction
|Sliding velocity in the second direction
|Dissipated energy in the first direction
|Dissipated energy in the second direction
! Definition of four nodes n1, n2, n3 and n4 explicitly
.NOE I n1 X - Y - Z -
I n2 X - Y - Z -
I n3 X - Y - Z -
I n4 X - Y - Z -
! or from points
.3PO I 1 X - Y - Z -
I 2 X - Y - Z -
I 3 X - Y - Z -
I 4 X - Y - Z -
.NOE I n1 POINT 1
I n2 POINT 2
I n3 POINT 3
I n4 POINT 4
! Definition of one contact element between the node N1 and
! the facet defined by the three nodes N2, N3 and N4.
.MCE I - CONT N n1 n2 n3 n4
! The positive normal to the facet is defined by the order of the nodes N2, N3 and N4
! following the corkscrew rule.
! Storage selection of the normal distance and the contact force between the node N1
! and the facet to plot a curve.
.SAI ARCH ELEM I - COMP 1 4
See here the list of keywords relating to the CONT element.
© 2018 Siemens Industry Software NV
Last update: 3-Jul-2018
If you have any suggestions or comments, please e-mail to the Webmaster