CONTPRM

Format

Example

Definitions

Parameters for OptiStruct Analysis

Parameters for Explicit Dynamic Analysis via Radioss Integration (ANALYSIS = EXPDYN)

Comments

1. The initial gap opening is calculated automatically based on the relative location of secondary and main nodes (in the original, undeformed mesh). To account for additional material layers covering main or secondary objects (such as half of shell thickness), the GPAD entry can be used. GPAD option THICK automatically accounts for shell thickness on both sides of the contact interface (this also includes the effects of shell element offset ZOFFS or composite offset Z0).
2. Option STIFF=AUTO determines the value of normal stiffness for each contact element using the stiffness of surrounding elements. Additional options SOFT and HARD create respectively softer or harder penalties. SOFT can be used in cases of convergence difficulties and HARD can be used if undesirable penetration is detected in the solution. A negative value for STIFF indicates that a stiffness scaling factor equal to |Real < 0.0| is defined. This scaling is applied on the stiffness value via STIFF = AUTO.
3. MU1=STICK is interpreted in OptiStruct as an enforced stick condition - such contact interfaces will not enter the sliding phase. Of course, the enforced stick only applies to contacts that are closed.
4. MU1=FREEZE enforces zero relative displacements on the contact surface - the contact gap opening remains fixed at the original value and the sliding distance is zero. The FREEZE condition applies to all secondary nodes, no matter whether their initial gap is open or closed.
5. The file filename_root.contgap.fem, produced using the CONTGAP parameter, can be imported into HyperMesh in order to visualize internally created node-to-surface contact elements (now converted to GAPG entities).
   Note: During optimization, this file shows node-to-surface contact elements for the latest optimization iteration. In order to correctly visualize this configuration in HyperMesh for shape optimization problems, the FEA mesh shape needs to be updated by applying "Shape change" results.

   Furthermore, if GAPPRM,HMGAPST,YES is activated together with CONTPRM,CONTGAP,YES, then the gap status command file, filename_root.HM.gapstat.cmf, will also include the open/closed status of these additional GAPG's that represent node-to-surface contact elements. For correct visualization of their status in HyperMesh, file filename_root.contgap.fem needs to be imported before running the gap status command file.

6. Adaptive contact penalty is not applicable to these cases:
   • TIE or FREEZE contact
   • Contact with nonlinear penalty
   • No-separation contact
7. The maximum allowed penetration for adaptive contact penalty is selected as MAXPNTR*L.

   Where, L is the characteristic edge length (the average edge length on the main surface) of the contact.

8. The initial trial penalty for adaptive contact penalty is selected as:
   • KA0TUNE*K

     Where, K is an automatically selected raw stiffness value, if STIFF=AUTO for the contact interface.

   • The contact penalty stiffness value of STIFF option, otherwise.
9. If ISTF ≠ 1, the interface stiffness K is computed from the main segment stiffness Km and/or the secondary segment stiffness Ks.

   The main stiffness is computed from $Km=STFAC\cdot B\cdot S\cdot \raisebox{1ex}{$S$}\!\left/ \!\raisebox{-1ex}{$V$}\right.$ for solids, $Km=0.5\cdot STFAC\cdot E\cdot t$ for shells as well as when the main segment is shared by a shell and a solid.

   The secondary stiffness is an equivalent nodal stiffness computed as for solids: (1)

   $$Ks=STFAC\cdot B\cdot V^{-3}$$

   For Shells:(2)

   $$Ks=0.5\cdot STFAC\cdot E\cdot t$$
   Where,

   $B$

   Bulk modulus

   $S$

   Segment area

   $E$

   Modulus of elasticity

   $t$

   Shell thickness

   $V$

   Volume of a solid

   There is no limitation to the value of stiffness factor (but a value greater than 1.0 can reduce the initial time step).

   ISTF = 0, the interface stiffness $K=Km$

   ISTF > 1, the interface stiffness is $K=\max \left(STMIN,\min \left(STMAX,K1\right)\right)$ with:

   • ISTF = 2, $K1=0.5\cdot \left(Km+Ks\right)$
   • ISTF = 3, $K1=\max \left(Km,Ks\right)$
   • ISTF = 4, $K1=\min \left(Km,Ks\right)$
   • ISTF = 5, $K1=Km\cdot Ks/\left(Km+Ks\right)$
10. In an implicit analysis, the contact stiffness plays a very important role in convergence. ISTF = 4 (which takes the minimum of main and secondary stiffness's for contact) is recommended. This is because the penalty contact force will be balanced with the internal force of the deformable impacted part, which means the stiffness near the effective stiffness one will converge easier than a higher one.

    For small initial gaps in implicit analysis, the convergence will be more stable if a GAP larger than the initial gap is defined.

    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.

11. The default for the constant gap (IGAP = CONST) is the minimum of:

    t

    Average thickness of the main shell elements

    l/10, l

    Average side length of the main solid elements

    lmin/2, lmin

    Smallest side length of all main segments (shell or solid)

12. The variable gap (IGAP = VAR) is computed as gs + gm with:
    • gm - main element gap with
      • gm = t/2, t: thickness of the main element for shell elements.
      • gm = 0 for solid elements.
    • gs - secondary node gap:
      • gs = 0 if the secondary 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 secondary node.
      • gs = 1/2√S for truss and beam elements, with S being the cross-section of the element.

    If the secondary node is connected to multiple shells and/or beams or trusses, the largest computed secondary gap is used.

    The variable gap is always at least equal to GAPMIN.

13. INACTI = 3 or 4 are only recommended for small initial penetrations and should be used with caution because:
    • the coordinate change is irreversible
    • it may create other initial penetrations if several surface layers are defined in the interfaces
    • it may create initial energy if the node belongs to a spring element
    INACTI = 5 works as:

    Figure 1.

14. IFILT defines the method for computing the friction filtering coefficient. If IFILT ≠ NO, the tangential friction forces are smoothed using a filter:(3)
    $$F_T=\alpha \cdot F{\text{'}}_T+\left(1-\alpha \right)\cdot F{\text{'}}_{T-1}$$
    Where,

    $F_T$

    Tangential force

    $F{\text{'}}_T$

    Tangential force at time $t$

    $F{\text{'}}_{T-1}$

    Tangential force at time $t-1$

    α

    Filtering coefficient

    IFILT = SIMP

    α = FFAC

    IFILT = PER

    $\alpha =2\pi dt/FFAC$ , where dt/T = FFAC, $T$ is the filtering period

    IFILT = CUTF

    $\alpha =2\pi \cdot FFAC\cdot dt$ , where FFAC is the cutting frequency

15. IFRIC defines the friction model.

    IFRIC = COUL - Coulomb friction with $F_T\le \mu \cdot F_N$ with $\mu =FRIC$

    If IFRIC is not COUL, the friction coefficient is set by a function $\left(\mu =\mu \left(p,V\right)\right)$ ,

    Where,

    $p$

    Pressure of the normal force on the main segment

    $V$

    Tangential velocity of the secondary node

    The following formulations are available:

    IFRIC = GEN - Generalized viscous friction law(4)

    $$\mu =Fric+C_1\cdot p+C_2\cdot V+C_3\cdot p\cdot V+C_4\cdot p^2+C_5\cdot V^2$$
    IFRIC = DARM - Darmstad law(5)

    $$\mu =C_1\cdot e^{\left(C_{2}V\right)}\cdot p^2+C_3\cdot e^{\left(C_{4}V\right)}\cdot p+C_5\cdot e^{\left(C_{6}V\right)}$$
    IFRIC = REN - Renard law(6)

    $$\mu =C_1+(C_3-C_1)\cdot \frac{V}{C_5}\cdot \left(2-\frac{V}{C_5}\right)\mathit{if}V\in \left[0,C_5\right]$$

    (7)

    $$\mu =C_3-((C_3-C_4)\cdot {\left(\frac{V-C_5}{C_6-C_5}\right)}^2\cdot \left(3-2-\frac{V-C_5}{C_6-C_5}\right))\mathit{if}V\in \left[C_5,C_6\right]$$

    (8)

    $$\mu =C_2-\frac{1}{\frac{1}{C_2-C_4}+{\left(V-C_6\right)}^2}\mathit{if}\hspace{0.17em}V\ge C_6$$

    where,

    $\begin{array}{l}{C}_1=C1={\mu }_S,C_2=C2={\mu }_d\\ C_3=C3={\mu }_{\text{max}},C_4=C4={\mu }_{\text{min}}\\ C_5=C5=V_{cr1},C_6=C6=V_{cr2}\end{array}$

    • The first critical velocity $V_{cr1}$ must be different to 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 the maximum friction C3 (C1 ≤ C3) and C2 ≤ C3).
    • The minimum friction coefficient C4, must be lower than the static friction coefficient C1 and the dynamic friction coefficient C2 (C4 ≤ C1 and C4 ≤ C2).
16. IFORM selects two types of contact friction penalty formulation.
    The viscous (total) formulation (IFORM = VISC) computes an adhesive force as:(9)

    $$F_{adh}=VISF\cdot Sqrt\left(2Km\right)\cdot V_T{F}_T=\min \left(\mu F_N,F_{adh}\right)$$
    The stiffness (incremental) formulation (IFORM = STIFF) computes an adhesive force as:(10)

    $$F_{adh}=F_{Told}+\text{Δ}{F}_T$$

    (11)

    $$\text{Δ}{F}_T=K\cdot V_T\cdot dt$$

    (12)

    $$F_{Tnew}=\min \left(\mu F_N,F_{adh}\right)$$
17. For nonlinear implicit contact with friction, the stiffness formulation (IFORM = STIFF) is recommended.
18. If IGNORE = 1 or 2, the secondary nodes without a main segment found during the searching are deleted from the interface.

    If IGNORE = 1 and SRCHDIS is blank, the default value of the distance for searching closest main segment is the average size of the main segments.

    If IGNORE = 2 and SRCHDIS is blank, the distance for searching closest main segment for each secondary node is computed as:

    $d_1=0.6\cdot \left(T_s+T_m\right)$

    $d_2=0.05\cdot T_{md}$

    $SRCHDIS=\max \left(d_1,d_2\right)$

    Where,

    $T_s$

    Thickness of the element connected to the secondary node, for solids $T_s$ = 0.0

    $T_m$

    Thickness of main segment, for solids $T_m$ = Element volume / Segment area

    $T_{\mathrm{md}}$

    Main segment diagonal

19. This card is represented as a control card in HyperMesh.