This section describes user subroutines that you can use to customize contact interfacial behavior for contact elements (CONTA171 to CONTA178). These subroutines allow you to:
Perform a user-defined operation on real constants (subroutine usercnprop
)
Write your own friction laws (subroutine
userfric
)
Write your own contact interactions (subroutine userinter
)
Write your own wear law (subroutine
userwear
)
This subroutine applies to the CONTA17x contact
elements.
*deck,usercnprop USERSDISTRIB
subroutine usercnprop (ndim,coor,nkeyopt,keyopt,nrl,rlconst,
x nintIn,intIn,nrealIn,realIn,kupdhis,localr,nuval,nintp,usvr,
x ncomp,stress,strain0,strain,kstat,mu,kcnprop,cnprop,keyerr)
c
c *** primary function: Allow users to define their own contact properties
c in real constant table
c This logic is accessed with real constant defined
c by table name: %_CNPROP%
c (e.g. rmod,cid,kcnprop,%_CNPROP%)
c
c *** Notice - This file contains ANSYS Confidential information ***
c
c
c Copyright ANSYS. All Rights Reserved.
c *** ansys, inc.
c
c input arguments:
c variable (type,sze,intent) description
c
c elem (int,sc,in) - element number
c intpt (int,sc,in) - element integration point number
c ndim (int,sc,in) - number of dimensions of the problem
c = 2 2D
c = 3 3D
c nintp (int,sc,in) - the total number of integration points of
c an element to be used with this routine
c nuval (int) - number of additional state variables per
c integration point
c note: nuval x nintp = nstv(on nsvr command); cannot exceed 840!
c
c intIn (int,ar(*),in) - integer variables passed in
c intIn (int,ar(*),in) - integer variables passed in
c intIn(1) = element number
c intIn(2) = element integration point number
c intIn(3) = material reference number
c intIn(4) = element type ID number (absolute value)
c > 0 for CONTA171-CONTA177
c < 0 for CONTA178
c intIn(5) = real constant ID number
c intIn(6) = associated contact nodal number
c intIn(7) = contact indicator
c 0: intersection is found
c otherwise: no intersection
c intIn(8) = target element number
c intIn(9) = flag for forcing sliding
c frictional case
c 0 : not forcing
c 1 : forcing (Slip direction is
c defined through CMROT command)
c intIn(10) = 1 first pass through
c (1st iteration)
c (useful for initializing state
c variables to a non-zero value)
c = 2 first pass through key of
c a restart
c = 3 first pass through key of
c a rezoning
c intIn(11) = current load step number
c intIn(12) = current substep number
c intIn(13) = current equilibrium iteration
c number
c intIn(14) = flag for using unsymmetric
c matrices (nropt,unsym)
c 0 : symmetric
c 1 : unsymmetric
c intIn(15) = Linear perturbation flag
c 0 : a general load step
c 1 : a linear perturbation step
c intIn(16) = key to indicate output pass
c 0 : not a output pass
c 1 : output pass
c intIn(17) = key to indicate if history-
c dependent variables
c (user defined) need to be
c updated after the substep has
c converged
c 1 : update (converged)
c 0 : do not update (not converged)
c intIn(18) = key to indicate transient effects
c 1 : transient is active
c 0 : transient is not active
c intIn(19) = large deformation key [nlgeom cmd]
c 1 : on
c 0 : off
c intIn(20) = analysis type (derived from
c antype cmd)
c 0 : a static analysis
c 1 : a buckling analysis
c 2 : a modal analysis
c 3 : a harmonic analysis
c 4 : a transient analysis
c 7 : a substructure analysis
c 8 : a spectrum analysis
c intIn(21) = key for displacement & force
c convergence
c 1 : converged
c 0 : not converged
c realIn (dp,ar(*),in) - real variables passed in
c realIn(1) = contact element length
c realIn(2) = contact element depth
c realIn(3) = area associated with the contact
c detection point
c realIn(4) = pinball radius
c realIn(5) = un-scaled normal penalty stiffness
c realIn(6) = time (or frequency for a harmonic
c analysis) at the beginning of this
c load step
c realIn(7) = time (or frequency for a harmonic
c analysis) at the end of this load step
c realIn(8) = current time value (or frequency value
c for a harmonic analysis)
c realIn(9) = time increment (or frequency increment
c for a harmonic analysis) over this
c substep
c realIn(10)= temperature offset from absolute
c zero
c realIn(11)= geometric penetration/gap
c (current substep)
c > 0 : gap
c < 0 : penetration
c realIn(12)= time increment scaling factor to
c be used for structural transient
c dynamics
c nkeyopt (int,sc,in) - number of key options
c keyopt (int,ar(nkeyopt),in)- array containing key options
c keyopt(1) : Select degree of freedom
c keyopt(2) : Contact algorithm
c ... so on (see ANSYS documentation)
c nrl (int,sc,in) - number of real constants
c rlconst (dp,ar(nrl),in) - array containing real constants
c Elements CONTA171 to CONTA177
c rlconst(1) : R1
c rlconst(2) : R2
c rlconst(3) : FKN
c rlconst(4) : FTOLN
c ... so on (see ANSYS documentation)
c Element CONTA178
c rlconst(1) : FKN
c rlconst(2) : GAP
c ... so on (see ANSYS documentation)
c
c kcnprop (int,sc,in) - the position of constant in the real set
c
c (see ANSYS contact element manual)
c ncomp (int,sc,in) - number of stress/force component
c = 9 for CONTA171-CONTA177
c = 7 for CONTA178
c stress (dp,ar(ncomp),in) - stress components at the beginning of
c the current iteaation/substep.
c stress(1) = frictional stress in direction 1
c stress(2) = frictional stress in direction 2
c (3D only)
c stress(3) = contact normal pressure
c > 0 : compression
c < 0 : tension
c the above contact traction must be defined in
c a local coordinate system (see localr)
c stress(4) = heat flux (per area)
c flowing into contact
c stress(5) = heat flux (per area)
c flowing into target
c < 0 heat flowing into a surface
c > 0 heat flowing out of a surface
c stress(6) = electrical current density
c (or pore fluid flux density)
c (per area) flowing into contact
c stress(7) = electrical current density
c (or pore fluid flux density)
c (per area) flowing into target
c > 0 current flowing out of a surface
c < 0 current flowing into a surface
c stress(8) = diffusion flux density
c (per area) flowing into contact
c stress(9) = diffusion flux density
c (per area) flowing into target
c > 0 flux flowing out of a surface
c < 0 flux flowing into a surface
c strain0 (dp,ar(ncomp),in) - strain components in the end of the previous
c substep
c (see strain for each component definition)
c strain (dp,ar(ncomp),in) - current strain components
c strain(1) = slip increment in direction 1
c strain(2) = slip increment in direction 2
c (3D only)
c strain(3) = contact normal gap/penetration
c < 0 : gap
c > 0 : penetration
c strain(4) = temperature at the contact point
c (from TEMP DOF or temperature load)
c strain(5) = temperature at the target point
c (only from TEMP DOF)
c strain(6) = voltage (or pore pressure)
c at the contact point
c strain(7) = voltage (or pore pressure)
c at the target point
c strain(8) = concentrationat the contact point
c strain(9) = concentrationat the target point
c kstat (int,sc,in) - contact status at the end of the previous
c substep
c 3 : stick
c 2 : sliding
c 1 : open contact (near)
c 0 : open contact (far)
c mu (dp,sc,in) - The frictional coef at the end of previous
c substep
c coor (dp,ar(6),in) - Coordinates of the contact detection point
c coor(1) current x
c coor(2) current y
c coor(3) current z
c coor(4) initial x
c coor(5) initial y
c coor(6) initial z
c localr (dp,ar(3,3),in) - the direction cosines of the local surface
c coordinate system at contact detection
c localr(1,1),localr(1,2),localr(1,3) in slip
c direction 1
c localr(2,1),localr(2,2),localr(2,3) in slip
c direction 2
c localr(3,1),localr(3,2),localr(3,3) in normal
c direction
c
c usvr (dp,ar(nuval,nintp),inout)- additional state variables from
c previous equilibrium iteration (saved
c if the nsvr command is used)
c kupdhis (int,sc,in) - key to indicate if history-dependent
c variables (user defined) need to be
c updated after the substep has converged
c 1 : update (converged)
c 0 : do not update (not converged)
c
c output arguments:
c variable (type,sze,intent) description
c cnprop (dp,ar(5),out) - user defined real constant value and
c derivatives w.r.t. kcnprop position
c cnprop(1) = user defined real constant value
c (e.g. kcnprop = 3 for normal contact
c stiffness FKN.
c positive as scaling factor;
c negative value as the absolute value)
c cnprop(2) = derivative of the real constant
c w.r.t. geometric penetration/gap
c cnprop(3) = derivative of the real constant
c w.r.t. contact normal pressure
c cnprop(4) = derivative of the real constant
c w.r.t. temperature at contact
c cnprop(5) = derivative of the real constant
c w.r.t. temperature at target
c usvr (dp,ar(nuval,nintp),inout)- updated additional state variables
c They are passed in as the values at the
c beginning of this substep.
c They are updated to be the values at the
c end of this substep
c Use NSVR command to size usvr array and
c set nuval to same value as number of
c variables on NSVR commands
c Use userou.F to save these values
c on NMISC record for output purposes.
c The number of user defined output items on
c NMISC should be equal or less than NSTV
c on nsvr command). It cannot exceed 120.
c
c keyerr (int,sc,inout) - key to indicate if there is any element
c formulation error.
c The error could be caused by too
c large incremental step, illegal model.
c = 0 no error (present value before calling)
c = 1 some error happens. ANSYS will
c decide to stop the analysis or cutback
c the substep (bi-section) based on other
c user input and information at higher
c level.
c
This subroutine applies to the CONTA17x contact
elements.
*deck,userfric USERSDISTRIB
subroutine userfric (elem,mat,intpt,nkeyopt,keyopt,nrl,rlconst,
x ncomp,npropu,uprop,kfirst,kfsteq,kn,kt,elen,kstat,timval,
x timinc,tcont,ttarg,toffst,dslip,slip,pres,tau,dt,usvr,
x fdiss,elener,kupdhis,mu,dtdp)
c
c *** primary function: Allow users to write their own friction laws.
c This logic is accessed with tb,fric with tbopt=user.
c The below demonstration logic is the same as using
c tb,fric for isotropic Coulomb friction.
c Other friction laws may require more general
c definition of friction forces.
c *** secondary function: demonstrate the use of user-written friction laws
c in this routine:
c a. update history variables
c b. compute consistent tangent matrix
c
c *** Notice - This file contains ANSYS Confidential information ***
c
c
c Copyright ANSYS. All Rights Reserved.
c *** ansys, inc.
c
c input arguments:
c variable (type,sze,intent) description
c
c elem (int,sc,in) - element number (label)
c mat (int,sc,in) - material reference number
c intpt (int,sc,in) - element integration point number
c nkeyopt (int,sc,in) - number of key options
c keyopt (int,ar(nkeyopt),in)- array containing key options
c keyopt(1) : Select degree of freedom
c keyopt(2) : Contact algorithm
c ... so on (see ANSYS documentation)
c nrl (int,sc,in) - number of real constants
c rlconst (dp,ar(nrl),in) - array containing real constants
c Elements CONTA171 to CONTA177
c rlconst(1) : R1
c rlconst(2) : R2
c rlconst(3) : FKN
c rlconst(4) : FTOLN
c ... so on (see ANSYS documentation)
c Element CONTA178
c rlconst(1) : FKN
c rlconst(2) : GAP
c ... so on (see ANSYS documentation)
c ncomp (int,sc,in) - no. of friction stress components (1 or 2)
c npropu (int,sc,in) - no. of user-defined friction properties
c uprop (dp,ar(npropu),in) - user-defined material properties
c kfirst (int,sc,in) - 1 if first time through, 0 otherwise
c (useful for initializing state variables
c to a non-zero value)
c kfsteq (int,sc,in) - 1 if first equilibrium iteration of a
c substep, 0 otherwise
c kn (dp,sc,in) - normal penalty stiffness
c kt (dp,sc,in) - tangential penalty stiffness
c (an initial guess is provided but
c the user must pick a suitable
c value that allows minimal tangential
c slip during sticking without
c adversely affecting the convergence;
c a possible choice could be kt=mu*kn).
c For Lagrange multiplier method (keyopt(2)=4
c use a small kt (several orders of magnitude
c smaller than mu*pres).
c elen (dp,sc,in) - length of contact element
c kstat (int,sc,inout) - contact status
c 3 : stick
c 2 : sliding
c 1 : open contact (near)
c 0 : open contact (far)
c timval (dp,sc,in) - current time value
c timinc (dp,sc,in) - time increment over this substep
c tcont (dp,sc,in) - contact surface temperature
c (from temperature DOF or temperature load)
c ttarg (dp,sc,in) - target surface temperature
c (only from temperature DOF)
c toffst (dp,sc,in) - temperature offset from absolute zero
c dslip (dp,ar(ncomp),in) - slip increment (current substep)
c slip (dp,ar(ncomp),inout)- accumulated slip (previous substep)
c pres (dp,sc,in) - normal pressure/force (current substep)
c > 0 : compression
c < 0 : tension
c tau (dp,ar(ncomp),inout)- frictional stress (previous substep)
c Lagrange multiplier contribution is added
c if keyopt(2)=4
c usvr (dp,ar(nuval,nintp),inout)- additional state variables from
c previous equilibrium iteration (saved
c if the nsvr command is used)
c kupdhis (int,sc,in) - key to indicate if history-dependent
c variables (user defined) need to be
c updated after the substep has converged
c 1 : update (converged)
c 0 : do not update (not converged)
c
c output arguments:
c variable (type,sze,intent) description
c
c kstat (int,sc,inout) - updated contact status
c mu (dp,sc inout) - updated friction coefficient
c slip (dp,ar(ncomp),inout)- updated accumulated slip
c tau (dp,ar(ncomp),inout)- updated frictional stress
c dt (dp,ar(5,5),out) - material tangent modulus
c rows and columns of dt matrix are
c associated to:
c row 1 : frictional stress in direction 1
c row 2 : frictional stress in direction 2
c row 3 : normal pressure
c row 4 : blank
c row 5 : blank
c col 1 : sliding in direction 1
c col 2 : sliding in direction 2
c col 3 : normal gap
c col 4 : temperature at contact
c col 5 : temperature at targte
c relevant components to be filled in are:
c dt(1,1): d(tau1)/d(slip1)
c dt(1,2): d(tau1)/d(slip2)
c dt(1,3): d(tau1)/d(normal gap)
c dt(2,1): d(tau2)/d(slip1)
c dt(2,2): d(tau2)/d(slip2)
c dt(2,3): d(tau2)/d(normal gap)
c dt(3,3): d(pres)/d(normal gap)
c dt(3,3) set to kn internally
c dt(1,4) : d(tau1)/d(tcont)
c dt(1,5) : d(tau1)/d(ttarg)
c dt(2,4) : d(tau2)/d(tcont)
c dt(2,5) : d(tau2)/d(ttarg)
c dtdp (dp,ar(ncomp),out) - partial derivative of the frictional
c stress in direction 1/2 w.r.t. normal
c pressure used in Lagrange multiplier
c method (keyopt(2)=3,4).
c usvr (dp,ar(nuval,nintp),inout)- updated additional state variables
c For example, mu value and absolute
c accumulated slip could be output as follows:
c usvr(1,intpt) : mu
c usvr(2,intpt) : abs. acc. slip in dir1
c usvr(3,intpt) : abs. acc. slip in dir2
c Use NSVR command to size usvr array and
c set nuval to same value as number of
c variables on NSVR commands
c Use userou.F to save these values
c on NMISC record for output purposes.
c The number of user defined output items on
c NMISC should be equal or less than NSTV
c on nsvr command). It cannot exceed 120.
c
c fdiss (dp,sc,out) - incremental frictional dissipation
c per unit area
c elener (dp,sc,out) - incremental elastic stored energy
c per unit area
c
c fortran parameters (to be defined by the user):
c variable (type) description
c nuval (int) - number of additional state variables per
c integration point
c nintp (int) - maximum number of integration points of
c an element to be used with this routine
c (14 is the maximum)
c note: nuval x nintp = nstv(on nsvr command); cannot exceed 840!
c
c internal variables:
c variable (type,sze) description
c dtfac (dp,sc) - temporary variable
c taulim (dp,sc) - limit frictional stress
c taueq (dp,sc) - equivalent frictional stress
c dir1 (dp,sc) - slip increment direction 1
c dir2 (dp,sc) - slip increment direction 2
c dslipeq (dp,sc) - equivalent slip increment
c oldt1 (dp,sc) - frictional stress 1 from prev substep
c oldt2 (dp,sc) - frictional stress 2 from prev substep
c err (dp,ar(2)) - data array for diagnostic message
c
This subroutine applies to the CONTA17x contact
elements.
*deck,userinter USERSDISTRIB
subroutine userinter (ndim,coor,nkeyopt,keyopt,nrl,rlconst,
x npropu,uprop,nintIn,intIn,nrealIn,realIn,kupdhis,localr,
x nuval,nintp,usvr,ncomp,stress,strain0,strain,
x kstat,mu,dt,dtdp,kdamp,damp,fdiss,elener,keyerr,keycnv)
c
c *** primary function: Allow users to write their own interaction behavior.
c This logic is accessed with tb,inter with tbopt=user.
c *** secondary function: demonstrate the use of user-written interface laws
c in this routine:
c a. update history variables
c b. compute consistent tangent matrix
c
c *** Notice - This file contains ANSYS Confidential information ***
c
c
c *** Copyright ANSYS. All Rights Reserved.
c *** ansys, inc.
c
c input arguments:
c variable (type,sze,intent) description
c
c elem (int,sc,in) - element number
c intpt (int,sc,in) - element integration point number
c ndim (int,sc,in) - number of dimensions of the problem
c = 2 2D
c = 3 3D
c nintp (int,sc,in) - the total number of integration points of
c an element to be used with this routine
c nuval (int) - number of additional state variables per
c integration point
c note: nuval x nintp = nstv(on nsvr command); cannot exceed 840!
c
c intIn (int,ar(*),in) - integer variables passed in
c intIn(1) = element number
c intIn(2) = element integration point number
c intIn(3) = material reference number
c intIn(4) = element type ID number (absolute value)
c > 0 for CONTA171-CONTA177
c < 0 for CONTA178
c intIn(5) = real constant ID number
c intIn(6) = associated contact nodal number
c intIn(7) = contact indicator
c 0: intersection is found
c otherwise: no intersection
c intIn(8) = target element number
c intIn(9) = flag for forcing sliding
c frictional case
c 0: - not forcing
c 1: - forcing (Slip direction is
c defined through CMROT command)
c intIn(10) = 1 first pass through
c (1st iteration)
c (useful for initializing state
c variables to a non-zero value)
c = 2 first pass through key of
c a restart
c = 3 first pass through key of
c a rezoning
c intIn(11) = current load step number
c intIn(12) = current substep number
c intIn(13) = current equilibrium iteration number
c intIn(14) = flag for using unsymmetric matrices
c (nropt,unsym)
c 0: - symmetric
c 1: - unsymmetric
c intIn(15) = Linear perturbation flag
c 0: - a general load step
c 1: - a linear perturbation step
c intIn(16) = key to indicate output pass
c 0: not a output pass
c 1: output pass
c intIn(17) = key for displacement & force
c convergence
c 1: converged
c 0: not converged
c intIn(18) = key to indicate transient effects
c 1 : transient is active
c 0 : transient is not active
c intIn(19) = large deformation key [nlgeom cmd]
c 1 : on
c 0 : off
c intIn(20) = analysis type (derived from antype)
c 0 : a static analysis
c 1 : a buckling analysis
c 2 : a modal analysis
c 3 : a harmonic analysis
c 4 : a transient analysis
c 7 : a substructure analysis
c 8 : a spectrum analysis
c realIn (dp,ar(*),in) - real variables passed in
c realIn(1) = contact element length
c realIn(2) = contact element depth
c realIn(3) = area associated with the contact
c detection point
c realIn(4) = pinball radius
c realIn(5) = unscaled normal penalty stiffness
c realIn(6) = time (or frequency for a harmonic
c analysis) at the beginning of this
c load step
c realIn(7) = time (or frequency for a harmonic
c analysis) at the end of this load step
c realIn(8) = current time value (or frequency value
c for a harmonic analysis)
c realIn(9) = time increment (or frequency increment
c for a harmonic analysis) over this
c substep
c realIn(10) = temperature offset from absolute
c zero
c realIn(11) = geometric penetration/gap
c (current substep)
c > 0 : gap
c < 0 : penetration
c realIn(12) = time increment scaling factor to
c be used for structural transient
c dynamics
c realIn(13) = convection coefficient (SFE command)
c realIn(14) = bulk temp (SFE command)
c nkeyopt (int,sc,in) - number of key options
c keyopt (int,ar(nkeyopt),in)- array containing key options
c keyopt(1) : Select degree of freedom
c keyopt(2) : Contact algorithm
c ... so on (see ANSYS documentation)
c nrl (int,sc,in) - number of real constants
c rlconst (dp,ar(nrl),in) - array containing real constants
c Elements CONTA171 to CONTA177
c rlconst(1) : R1
c rlconst(2) : R2
c rlconst(3) : FKN
c rlconst(4) : FTOLN
c ... so on (see ANSYS documentation)
c Element CONTA178
c rlconst(1) : FKN
c rlconst(2) : GAP
c ... so on (see ANSYS documentation)
c ncomp (int,sc,in) - number of stress/force component
c = 9 for CONTA171-CONTA177
c = 7 for CONTA178
c stress (dp,ar(ncomp),inout)- stress components (current substep)
c It is passed in as the stress at the beginning
c of the current substep. It is updated to be
c the stress at the end of this current substep
c stress(1) = frictional stress in direction 1
c stress(2) = frictional stress in direction 2
c (3D only)
c stress(3) = contact normal pressure
c > 0 : compression
c < 0 : tension
c the above contact traction must be defined in
c a local coordinate system (see localr)
c Lagrange multiplier contribution is added
c if keyopt(2)=3,4
c stress(4) = heat flux (per area)
c flowing into contact
c stress(5) = heat flux (per area)
c flowing into target
c < 0 heat flowing into a surface
c > 0 heat flowing out of a surface
c stress(6) = electrical current density
c (or pore fluid flux density)
c (per area) flowing into contact
c stress(7) = electrical current density
c (or pore fluid flux density)
c (per area) flowing into target
c > 0 current flowing out of a surface
c < 0 current flowing into a surface
c stress(8) = diffusion flux density
c (per area) flowing into contact
c stress(9) = diffusion flux density
c (per area) flowing into target
c > 0 flux flowing out of a surface
c < 0 flux flowing into a surface
c strain0 (dp,ar(ncomp),in) - strain components in the end of the previous
c substep
c (see strain for each component definition)
c strain (dp,ar(ncomp),in) - current strain components
c strain(1) = slip increment in direction 1
c strain(2) = slip increment in direction 2
c (3D only)
c strain(3) = contact normal gap/penetration
c < 0 : gap
c > 0 : penetration
c strain(4) = temperature at the contact point
c (from TEMP DOF or temperature load)
c strain(5) = temperature at the target point
c (only from TEMP DOF)
c strain(6) = voltage (or pore pressure)
c at the contact point
c strain(7) = voltage (or pore pressure)
c at the target point
c strain(8) = concentrationat the contact point
c strain(9) = concentrationat the target point
c
c kstat (int,sc,inout) - contact status (current substep)
c It is passed in as the status at the
c beginning of the current substep.
c It is updated to be the status at the
c end of the current substep
c 3 : stick
c 2 : sliding
c 1 : open contact (near)
c 0 : open contact (far)
c coor (dp,ar(6),in) - Coordinates of the contact detection point
c coor(1) current x
c coor(2) current y
c coor(3) current z
c coor(4) initial x
c coor(5) initial y
c coor(6) initial z
c localr (dp,ar(3,3),in) - the direction cosines of the local surface
c coordinate system at contact detection
c localr(1,1),localr(1,2),localr(1,3) in
c slip direction 1
c localr(2,1),localr(2,2),localr(2,3) in
c slip direction 2
c localr(3,1),localr(3,2),localr(3,3) in
c normal direction
c
c npropu (int,sc,in) - number of user-defined interaction properties
c uprop (dp,ar(npropu),in) - user-defined material properties
c
c usvr (dp,ar(nuval,nintp),inout)- additional state variables from
c previous equilibrium iteration (saved
c if the nsvr command is used)
c kupdhis (int,sc,in) - key to indicate if history-dependent
c variables (user defined) need to be
c updated after the substep has converged
c 1 : update (converged)
c 0 : do not update (not converged)
c
c output arguments:
c variable (type,sze,intent) description
c
c kstat (int,sc,inout) - updated contact status
c stress (dp,ar(ncomp),inout)- updated stress components
c
c dt (dp,ar(ncomp,ncomp),out)- interface stiffness matrix:
c dt(i,j) defines the partial derivative of
c the ith stress component at the current
c substep w.r.t. the jth component of the
c relative strain increment array.
c If symmetric solver option used, ANSYS will
c symmetrize the matrix bu averaging the
c off-diagonal terms.
c rows and columns of dt matrix are
c associated to:
c row 1 : frictional stress in direction 1
c row 2 : frictional stress in direction 2
c row 3 : normal pressure
c > 0 : compression
c < 0 : tension
c row 4 : heat flux out the contact surface
c < 0 heat flowing into contact
c > 0 heat flowing out of target
c row 5 : heat flux out the target surface
c < 0 heat flowing into target
c > 0 heat flowing out of target
c row 6 : electrical current density
c (or pore prssure)
c flowing out the contact surface
c > 0 current flowing out of contact
c < 0 current flowing into contact
c row 7 : electrical current density
c (or pore prssure)
c > 0 current flowing out of target
c < 0 current flowing into target
c row 8 : diffusion flux density
c flowing out the contact surface
c > 0 flux flowing out of contact
c < 0 flux flowing into contact
c row 9 : diffusion flux density
c > 0 flux flowing out of target
c < 0 flux flowing into target
c col 1 : sliding in direction 1
c col 2 : sliding in direction 2
c col 3 : normal gap
c < 0 : gap
c > 0 : penetration
c col 4 : temperature at the contact surface
c col 5 : temperature at the target surface
c col 6 : voltage at the contact surface
c col 7 : voltage at the target surface
c col 8 : concentration at the contact surface
c col 9 : concentration at the target surface
c relevant components to be filled in are:
c dt(1,1): d(tau1)/d(slip1)
c dt(1,2): d(tau1)/d(slip2)
c dt(1,3): d(tau1)/d(normal gap)
c dt(1,4): d(tau1)/d(tempC)
c dt(1,5): d(tau1)/d(tempT)
c dt(1,6): d(tau1)/d(voltC)
c dt(1,7): d(tau1)/d(voltT)
c dt(1,8): d(tau1)/d(concC)
c dt(1,9): d(tau1)/d(concT)
c dt(2,1): d(tau2)/d(slip1)
c dt(2,2): d(tau2)/d(slip2)
c dt(2,3): d(tau2)/d(normal gap)
c ...
c dt(3,1): d(pres)/d(slip 1)
c dt(3,2): d(pres)/d(slip 2)
c dt(3,3): d(pres)/d(normal gap)
c ...
c dt(4,1): d(fluxC)/d(slip 1)
c dt(4,2): d(fluxC)/d(slip 2)
c dt(4,3): d(fluxC)/d(normal gap)
c dt(4,4): d(fluxC)/d(tempC)
c dt(4,5): d(fluxC)/d(tempT)
c dt(4,6): d(fluxC)/d(voltC)
c dt(4,7): d(fluxC)/d(voltT)
c dt(4,8): d(fluxC)/d(concC)
c dt(4,9): d(fluxC)/d(concT)
c ...
c dt(5,4): d(fluxT)/d(tempC)
c dt(5,5): d(fluxT)/d(tempT)
c dt(5,6): d(fluxT)/d(voltC)
c dt(5,7): d(fluxT)/d(voltT)
c dt(5,8): d(fluxT)/d(concC)
c dt(5,9): d(fluxT)/d(concT)
c ...
c dt(6,4): d(eleC)/d(tempC)
c dt(6,5): d(eleC)/d(tempT)
c dt(6,6): d(eleC)/d(voltC)
c dt(6,7): d(eleC)/d(voltT)
c dt(6,8): d(eleC)/d(concC)
c dt(6,9): d(eleC)/d(concT)
c ...
c dt(7,4): d(eleT)/d(tempC)
c dt(7,5): d(eleT)/d(tempT)
c dt(7,6): d(eleT)/d(voltC)
c dt(7,7): d(eleT)/d(voltT)
c dt(7,8): d(eleT)/d(concC)
c dt(7,9): d(eleT)/d(concT)
c ...
c dt(8,4): d(diffC)/d(tempC)
c dt(8,5): d(diffC)/d(tempT)
c dt(8,6): d(diffC)/d(voltC)
c dt(8,7): d(diffC)/d(voltT)
c dt(8,8): d(diffC)/d(concC)
c dt(8,9): d(diffC)/d(concT)
c ...
c dt(9,4): d(diffT)/d(tempC)
c dt(9,5): d(diffT)/d(tempT)
c dt(9,6): d(diffT)/d(voltC)
c dt(9,7): d(diffT)/d(voltT)
c dt(9,8): d(diffT)/d(concC)
c dt(9,9): d(diffT)/d(concT)
c dtdp (dp,ar(ncomp),out) - partial derivative of the frictional stress
c in direction 1,2 w.r.t. normal pressure
c used in Lagrange multiplier method
c (keyopt(2)=3,4).
c damp (dp,ar(3,3),out) - interface damping matrix (structure only)
c it can be used only in Linear perturbation
c modal analysis or transient analysis or
c harmonic analysis in frequence domain.
c damp(i,j) defines the partial derivative of
c the ith stress component at the current
c substep w.r.t. the jth component of the
c strain increment rate array.
c rows and columns of dt matrix are
c associated to:
c row 1 : frictional stress in direction 1
c row 2 : frictional stress in direction 2
c row 3 : normal pressure
c col 1 : sliding rate in direction 1
c col 2 : sliding rate in direction 2
c col 3 : normal gap rate
c kdamp (int,sr,out) - damping matrix index
c 0 : no damping matrix
c 1 : taking damping matrix into account
c usvr (dp,ar(nuval,nintp),inout)- updated additional state variables
c For example, mu value and absolute/relative
c accumulated slip could be output as follows:
c usvr(1,intpt) : mu
c usvr(2,intpt) : abs. acc. slip in dir1
c usvr(3,intpt) : abs. acc. slip in dir2
c usvr(4,intpt) : acc. slip in dir1
c usvr(5,intpt) : acc. slip in dir2
c They are passed in as the values at the
c beginning of this substep. They are updated
c to be the values at the end of this substep.
c Use NSVR command to size usvr array and
c set nuval to same value as number of
c variables on NSVR commands
c Use userou.F to save these values
c on NMISC record for output purposes.
c The number of user defined output items on
c NMISC should be equal or less than NSTV
c on nsvr command). It cannot exceed 120.
c
c mu (dp,sc,inout) - The current frictional coefficient
c fdiss (dp,sc,out) - incremental frictional dissipation
c per unit area
c elener (dp,sc,out) - incremental elastic stored energy
c per unit area
c
c keyerr (int,sc,out) - key to indicate if there is any element
c formulation error, like
c contact status changes abruptly,
c too much penetration.
c The error could be caused by too
c large incremental step, illegal model.
c = 0 no error (preset value before calling)
c = 1 some error happens. ANSYS will
c decide to stop the analysis or cutback
c the substep (bi-section) based on other
c user input and information at higher
c level.
c keycnv (int,sc,inout) - key to flag if this element satisfies
c the user defined element convergence
c criterion.
c = 1, yes, the criterion is satisfied
c or don't have any criterion at all
c it is preset value before calling
c = 0, no, the element doesn't satisfy
c element convergence criterion. If
c this is the case, the iteration will
c not converge even when both force
c and displacement converge
c
c internal variables:
c variable (type,sze) description
c
This subroutine applies to contact elements CONTA171 - CONTA175.
*deck,userwear USERSDISTRIB
subroutine userwear(WearInc,WearDir,TotWearOld,strain,
x stress,temperature,dtime,YieldStress,nTbprop,Tbprop,
x coor,kstat,elem,intpt,ndim,localr)
c *** Primary Function: Calculates the Wear Increment and (optionally) wear direction
c *** Notice - This file contains ANSYS Confidential information ***
c
c
c *** Copyright ANSYS. All Rights Reserved.
c *** ansys, inc.
c input arguments:
c variable (type,sze,intent) description
c
c ndim (int,sc,in) - number of dimensions of the problem
c = 2 2D
c = 3 3D
c TotWearOld(dp,ar(ndim),in) - Total Wear at the contact point at the previous substep
c strain (dp,ar(3),in) - current strain components in contact surface coordinate system
c strain(1) = slip increment in direction 1
c strain(2) = slip increment in direction 2
c (3D only)
c strain(3) = contact normal gap/penetration
c < 0 : gap
c > 0 : penetration
c stress (dp,ar(3),in) - stress components in contact surface coordinate system
c stress(1) = frictional stress in direction 1
c stress(2) = frictional stress in direction 2
c (3D only)
c stress(3) = contact normal pressure
c > 0 : compression
c < 0 : tension
c temperature (dp,sc,in) - temperature
c dtime (dp,sc,in) - time increment
c YieldStress (dp,sc,in) - Yield stress of underlying element (defined only for Plastic material-see doc for restrictions)
c nTbprop (int,sc,in) - Number of TBdata for Tb,Wear per field
c Tbprop (dp,ar(nTbprop,in) - TB data for the the Tb,Wear option at the given temperature
c coor (dp,ar(6),in) - Coordinates of the contact detection point
c coor(1) current x
c coor(2) current y
c coor(3) current z
c coor(4) initial x
c coor(5) initial y
c coor(6) initial z
c kstat (int,sc,in) - contact status (current substep)
c 3 : stick
c 2 : sliding
c 1 : open contact (near)
c 0 : open contact (far)
c elem (int,sc,in) - element number
c intpt (int,sc,in) - element integration point number
c localr (dp,ar(3,3),in) - the direction cosines of the local surface
c coordinate system at contact detection
c localr(1,1),localr(1,2),localr(1,3) in
c slip direction 1
c localr(2,1),localr(2,2),localr(2,3) in
c slip direction 2
c localr(3,1),localr(3,2),localr(3,3) in
c normal direction
c Output Arguments:
c variable (type,sze,intent) description
c
c WearInc (dp,sc) - Increment in the Wear (magnitude)- User must define
c WearDir (dp,ar(ndim),inout) - Direction cosines in global coordinate system
c in which wear increment will be applied- Optional
c default coming in -Contact normal direction