PCNTX24

Format

Example

Definitions

Comments

1. The property identification number must be that of an existing PCONT Bulk Data Entry. Only one PCNTX24 property extension can be associated with a particular PCONT.
2. PCNTX24 is only supported for geometric nonlinear explicit dynamic analysis subcase defined by ANALYSIS = EXPDYN. It is ignored for all other subcases.
3. If FRIC is not explicitly defined on the PCONTX/PCNTX# entries, the MU1 value on the CONTACT or PCONT entry is used for FRIC in the /INTER entries for Geometric Nonlinear Analysis. Otherwise, FRIC on PCONTX/PCNTX# overwrites the MU1 value on CONTACT/PCONT.
4. In implicit analysis, different contact formulations are used for contact where slave and master set do not overlap and where they overlap (self-contact).

   In the case of self-contact, the gap cannot be zero and a constant gap is used. For small initial gaps, the convergence will be more stable and faster if GAP is larger than the initial gap.

   In implicit analysis, sometimes a stiffness with scaling factor reduction (for example, STFAC = 0.01) or reduction in impacted thickness (if rigid one) might reduce unbalanced forces and improve convergence, particularly in shell structures under bending where the effective stiffness is much lower than membrane stiffness; but it should be noted that too low of a value could also lead to divergence.

5. If ISTF ≠ 1, the interface stiffness K is computed from the master segment stiffness Km and/or the slave segment stiffness Ks.

   The master stiffness is computed from Km = STFAC * B * S * S/V for solids, Km = 0.5 * STFAC * E * t for shells.

   The slave stiffness is an equivalent nodal stiffness computed as Ks = STFAC * B * V^-3 for solids, Ks = 0.5 * STFAC* E * t for shells.

   In these equations, B is the Bulk Modulus, S is the segment area, and V is the volume of a solid. There is no limitation to the value of stiffness factor (but a value larger than 1.0 can reduce the initial time step).

   The interface stiffness is K = max (STMIN, min (STMAX, K1)) with:

   • ISTF = 0, K1 = Km
   • ISTF = 2, K1 = 0.5 * (Km + Ks)
   • ISTF = 3, K1 = max (Km, Ks)
   • ISTF = 4, K1 = min (Km, Ks)
   • ISTF = 5, K1 = Km * Ks / (Km + Ks)
6. The gap is computed automatically (similar with IGAP = VAR on PCNTX7) for each impact as gs + gm;
   with:

   • gm - master element gap, with:

     gm = t/2, t: thickness of the master element for shell elements.

     gm = 0 for solid elements.

   • gs - slave node gap:

     gs = 0 if the slave node is not connected to any element or is only connected to solid or spring elements.

     gs = t/2, t - largest thickness of the shell elements connected to the slave node.

     gs = 1/2✓S for truss and beam elements, with S being the cross section of the element.

   gm and gs are limited separately by GAPMAXm and GAPMAXs before the gap computation.

7. The coefficients C1 - C6 are used to define a variable friction coefficient $\mu$ .
8. IFRIC defines the friction model.

   IFRIC = COUL - Coulomb friction with F_T ≤ FRIC * F_N.

   For IFRIC > 0 the friction coefficient is set by a function ( $\mu =\mu (p,V)$ )

   Where, p is the pressure of the normal force on the master segment and V is the tangential velocity of the slave node.

   The following formulations are available:

   • IFRIC = GEN - Generalized viscous friction law(1)
     $$\mu =\text{FRIC}+\text{C}1*\text{p}+\text{C}2*\text{V}+\text{C}3*\text{p}*\text{v}+\text{C}4*{\text{p}}^2+\text{C}5*{\text{v}}^2$$
   • IFRIC = DARM - Darmstad law(2)
     $$\mu ={\text{C}}_1*\text{e}({\text{C}}_2\text{V})*{\text{p}}^2+{\text{C}}_3*\text{e}({\text{C}}_4\text{V})*\text{p}+{\text{C}}_5*\text{e}({\text{C}}_6\text{V})$$
   • IFRIC = REN - Renard law

     $\mu =C_1+\left(C_3-C_1\right)\cdot \frac{V}{C_5}\cdot \left(2-\frac{V}{C_5}\right)$	0 ≤ V ≤ C5
     $\mu =C_3-\left(\left(C_3-C_4\right)\cdot {\left(\frac{V-C_5}{C_6-C_5}\right)}^2\cdot \left(3-2\cdot \frac{V-C_5}{C_6-C_5}\right)\right)$	C5 ≤ V ≤ C6
     $\mu =C_2-\frac{1}{\frac{1}{C_2-C_4}+{\left(V-C_6\right)}^2}$	C6 ≤ V

     Where,(3)

     $$\begin{array}{l}{C}_1=C1={\mu }_s,C_2=C2={\mu }_d\hfill \\ C_3=C3={\mu }_{\text{max}},C_4=C4={\mu }_{\text{min}}\hfill \\ C_5=C5=V_{\mathit{cr}1},C_6=C6=V_{\mathit{cr}2}\hfill \end{array}$$
   • The first critical velocity V_cr1 must not be 0 (C5 ≠ 0). It also must be lower than the second critical velocity V_cr2 (C5 < C6).
   • The static friction coefficient C1 and the dynamic friction coefficient C2, must be lower than or equal to the maximum friction C3 (C1 ≤ C3 and C2 ≤ C3).
   • The minimum friction coefficient C4, must be lower than or equal to the static friction coefficient C1 and the dynamic friction coefficient C2 (C4 ≤ C1 and C4 ≤ C2).
9. IFILTR defines the method for computing the friction filtering coefficient. If IFILTR ≠ NO, the tangential friction forces are smoothed using a filter:

   F_T = α * F'_T + (1 - α) * F'_T-1

   Where,

   F_T

   Tangential force

   F'_T

   Tangential force at time t

   F'_T-1

   Tangential force at time t-1

   α

   Filtering coefficient

   IFILTR = SIMP - α = FFAC

   IFILTR = PER - α = 2π dt/FFAC, where dt/T = FFAC, T is the filtering period

   IFILTR = CUTF - α = 2π * FFAC * dt, where FFAC is the cutting frequency

10. IFORM selects two types of contact friction penalty formulation.

    The viscous (total) formulation (IFORM = VISC) computes an adhesive force as:

    F_adh = VISF * ✓(2KM) * V_T

    F_T = min ( $\mu$ F_N, F_adh)

    The stiffness (incremental) formulation (IFORM = STIFF) computes an adhesive force as:

    F_adh = F_Told + $\text{Δ}$ F_T

    $\text{Δ}$ F_T = K * V_T * dt

    F_Tnew = min ( $\mu$ F_N, F_adh)

11. When SENSID is defined for activation/deactivation of the interface, TSTART and TSTOP are not taken into account.
12. When the contact type is the symmetric surface to surface, the output normal contact forces in TH file are correctly calculated if the two surfaces are well separated.
13. For implicit test: Interface TYPE24 is now only available with SMP. The default of ISTF will be set to 4. The default INACTI will be set to -1.
14. This card is represented as an extension to a PCONT property in HyperMesh.