Erke_Wang-Ansys_Contact

Slide 1: 

ANSYS contact - Penalty vs. Lagrange - How to make it converge Erke Wang CAD-FEM GmbH. Germany

Slide 2: 

Variety of algorithms

Slide 3: 

Penalty means that any violation of the contact condition will be punished by increasing the total virtual work: Pure penalty method Augmented Lagrange method:

Slide 4: 

Pure penalty method The contact spring will deflect an amount , such that equilibrium is satisfied: Some finite amount of penetration, D > 0, is required mathematically to maintain equilibrium. However, physical contacting bodies do not interpenetrate (D = 0). There is no overconstraining problem Iterative solvers are applicable – large models are doable!

Slide 5: 

Pure penalty method Some finite amount of penetration, D > 0, is required mathematically to maintain equilibrium. However, physical contacting bodies do not interpenetrate (D = 0). Difference in d: 0.281e-3/ 0.284e-7 =1e4 Difference in stress: (3525-3501)/ 3525 =0.7% 100-times Difference in FKN leads to 100-times Difference in D but leads to only about 1% Difference in Contact pressure and the related stress.

Slide 6: 

Pure penalty method Some finite amount of penetration, D > 0, is required mathematically to maintain equilibrium. However, physical contacting bodies do not interpenetrate (D = 0). Tip: As long as the penetration does not leads to the change of the contact region, The penetration will not influence the contact pressure and Stress underneath the contact element Caution: For pre-tension problem, use large FKN>1, Because the small penetration will strongly influence the pre-tension force.

Slide 7: 

Pure penalty method The condition of the stiffness matrix crucially depends on the contact stiffness itself. If the contact stiffness is too large, it will cause convergence difficulties. The model can oscillate, with contacting surfaces bouncing off of each other. FKN=1 FKN=0.01

Slide 8: 

Pure penalty method The condition of the stiffness matrix crucially depends on the contact stiffness itself. This problem is almost solved since 8.1, with automatic contact stiffness adjustment. KEYOPT(10)=2

Slide 9: 

Pure penalty method The condition of the stiffness matrix crucially depends on the contact stiffness itself. For bending dominant problem, you should still use the 0.01 for the starting FKN and combine with KEYOPT(10)=2

Slide 10: 

Pure penalty method The condition of the stiffness matrix crucially depends on the contact stiffness itself. Tip: Always use KEYOPT(10)=2 For bending problem use FKN=0.01 and KEYOPT(10)=2 For bulky problem use FKN=1 and KEYOPT(10)=2 Caution: For pre-tension problem, use large FKN>1. Because the small penetration will strongly influence the pre-tension force.

Slide 11: 

Pure penalty method There is no additional DOF. There is no overconstraining problem Iterative solvers are applicable – large models are doable! Tip: Always use Penalty if: Symmetric contact or self-contact is used. Multiple parts share the same contact zone 3D large model(> 300.000 DOFs), use PCG solver.

Slide 12: 

Any violation of the contact condition will be furnished with a Lagrange multiplier. Pure Lagrange multipliers method Contact constraint condition: Ensure no penetration Ensure compressive contact force/pressure No contact , gap is non zero Contact , contact force is non zero The equation is linear, in case of linear elastic and Node-to-Node contact. Otherwise, the equation is nonlinear and an iterative method is used to solve the equation. Usually the Newton-Method is used. For linear elastic problems:

Slide 13: 

Pure Lagrange multipliers method Lagrange multipliers are additional DOFs  the FE model is getting large. Zero main diagonals in system matrix No iterative solver is applicable. For symmetric contact or additional CP/CE, and boundary conditions, the equation system might be over-constrained Sensitive to chattering of the variation of contact status No need to define contact stiffness Accuracy - constraint is satisfied exactly, there are no matrix conditioning problems

Slide 14: 

Pure Lagrange multipliers method Lagrange multipliers are additional DOFs  the FE model is getting large. Tip: Always use Lagrange multiplier method if: The model is 2D. 3D nonlinear material problem with < 100.000 Dofs

Slide 15: 

Pure Lagrange multipliers method Tip: If the Lagrange multiplier method is used: Always use asymmetric contact. Do not use CP/CE in on contact surfaces Do not define the multiple contacts, which share the common interfaces. For symmetric contact or additional CP/CE, and boundary conditions, the equation system is over-constrained Contact pair-1 Contact pair-1 Single contact pair

Slide 16: 

Pure Lagrange multipliers method Penalty symmetric Penetration Iterations: 174 CPU: 100 Pressure Lagrange symmetric Penetration Iterations: 92 CPU: 50 Pressure

Slide 17: 

Pure Lagrange multipliers method Tip: Use Penalty is chattering occurs or Chattering Control Parameters: FTOLN and TNOP Sensitive to chattering of the variation of contact status R1=R2-Delta R1 R2 F

Slide 18: 

Pure Lagrange multipliers method Penalty FKN=1 DELT=0.1 /prep7 et,1,183 et,2,169 et,3,172,,4,,2 mp,ex,1,2e5 pcir,190,200-DELT,-90,90 wpof,0,-delt pcir,200,210,-90,90 wpof,0,delt esiz,5 Esha,2 ames,all lsel,s,,,1 nsll,s,1 Real,2 type,3 esurf lsel,s,,,7 nsll,s,1 type,2 Esurf /solu Nsel,s,loc,x,0 D,all,ux lsel,s,,,5 nsll,s,1 d,all,all lsel,s,,,3 nsll,s,1 *get,nn,node,,count f,all,fy,200/nn alls Solv Use Penalty is chattering occurs

Slide 19: 

Pure Lagrange multipliers method Sy Pene Pure Penalty(FKN=1) Iter=8 No need to define contact stiffness Accuracy - constraint is satisfied exactly, there are no matrix conditioning problems

Slide 20: 

Pure Lagrange multipliers method Sy Pene Pure Lagrange Iter=13 Sy Pene Pure Penalty(FKN=1e4) Iter=39 No need to define contact stiffness Accuracy - constraint is satisfied exactly, there are no matrix conditioning problems

Slide 21: 

Pure Lagrange multipliers method example-1 Element: Plane183 Material: Neo-Hookean Contact: Pure Lagrange Load: Displacement

Slide 22: 

Pure Lagrange multipliers method /prep7 et,1,183 et,2,169 et,3,172,,3,,2 tb,hyper,1,,,neo tbdata,1,.3,0.001 mp,ex,2,2e5 mp,dens,2,7.8e-9 r,2,,,,,,5 r,3,,,,,,5 pcir,2,5 agen,5,1,1,,22 agen,2,1,1,,11,-30 agen,4,6,6,,22 rect,-6,-5,-80,0 rect,5,6,-30,0 agen,9,11,11,,11 pcir,5,6,0,180 agen,5,20,20,,22 wpof,11,-30 pcir,5,6,180,360 agen,4,25,25,,22 wpcs,-1 rect,-16,-6,-100,-80 rect,-6,-5,-100,-80 rect,-5,5,-100,-80 asel,s,,,10,31,1,1 numm,kp esha,2 esiz,2 ames,1,28 esha alls mat,2 ames,all lsel,s,,,74,106,8 lsel,a,,,80,112,8 lsel,a,,,115,131,4 lsel,a,,,133,145,4 nsll,s,1 type,2 real,2 mat,3 esurf lsel,s,,,1,4 lsel,a,,,9,12 lsel,a,,,17,20 lsel,a,,,25,28 lsel,a,,,33,36 cm,l1,line nsll,s,1 type,3 esurf lsel,s,,,76,108,8 lsel,a,,,78,102,8 lsel,a,,,113,129,4 lsel,a,,,135,147,4 nsll,s,1 type,2 real,3 esurf lsel,s,,,41,44 lsel,a,,,49,52 lsel,a,,,57,60 lsel,a,,,65,68 cm,l2,line nsll,s,1 type,3 esurf /solu nlgeo,on acel,,9810 asel,s,,,1,9,1,1 cmsel,u,l1 cmsel,u,l2 nsll,s,1 d,all,all asel,s,,,29,31,1 nsla,s,1 d,all,ux nsub,5,15,1 lsel,s,,,109,,,1 d,all,ux d,all,uy,0 alls cnvt,f,,.01 nsub,100,10000,1 solv lsel,s,,,109,,,1 d,all,uy,-50 nsub,100,10000,1 outres,all,all alls solv Tip: For large sliding problem, Use Lagrange method, the convergence behavior is very good and stable

Slide 23: 

Pure Lagrange multipliers method Lagrange: 110 Iterations CPU: 14 Sec. Penalty: 218 Iterations CPU: 24 Sec.

Slide 24: 

Pure Lagrange multipliers method Bending stress Contact penetration Bending example Lagrange: 10 Iterations 2 Sec. Penalty Key(10)=1: 54 Iterations 12 Sec.

Slide 25: 

Pure Lagrange multipliers method /prep7 et,1,183,,,1 et,2,183,,,1,,,1 et,3,169 et,4,172,,4,,2 mp,ex,1,2e5 tb,hyper,2,1,2,moon tbdata,1,1,.2,2e-3 Mp,mu,2,0.3 rect,1,5,0,3 rect,2,5,1.5,4 asba,1,2 rect,2.1,5,2.5,3.5 wpof,3,2 pcir,.501 esiz,.3 ames,1,3,2 esiz,.1 type,2 mat,2 ames,2 lsel,s,,,2 nsll,s,1 type,3 real,3 esurf lsel,s,,,8,12,4 nsll,s,1 type,4 esurf lsel,s,,,5 nsll,s,1 type,3 real,4 esurf lsel,s,,,13,14,1 nsll,s,1 type,4 esurf /solu nlgeo,on solcon,,,,1e-2 nsel,s,loc,y,0 d,all,uy nsel,s,loc,y,3.5 sf,all,pres,2 alls nsub,10,100,1 solv Rubber example Element: Plane183 Material: Mooney Contact: Pure Lagrange&Friction Load: Pressure Lagrange: 32 Iterations 13 Sec. Penalty Key(10)=2: 63 Iterations 20 Sec.

Slide 26: 

Pure Lagrange multipliers method /prep7 et,1,181 et,2,170 et,3,173,,3,,2 keyopt,3,11,1 mp,ex,1,2e5 r,1,.5 r,2,,,.1 r,3,,,.1 rect,0,10,0,5 agen,3,1,1,,,,0.5 esiz,1 esha,2 ames,all type,3 real,2 asel,s,,,1,,,1 esurf,,top type,2 asel,s,,,2,,,1 esurf,,bottom type,3 real,3 asel,s,,,2,,,1 esurf,,top type,2 asel,s,,,3,,,1 esurf,,bottom Shell example Element: Shell181 Material: elastic Contact: Pure Lagrange Load: Force /solu nlgeo,on nsel,s,loc,x,0 d,all,all nsel,s,loc,x,10 nsel,r,loc,y,5 nsel,r,loc,z,0 f,all,fz,1000 alls nsub,1,1,1 solv Lagrange: 15 Iterations 8 Sec. Penalty Key(10)=2: 18 Iterations 10 Sec.

Slide 27: 

Let us talk about convergence

Suggestion : 

One reason for convergence difficulties could be the following: FE Model is not modeled correctly in a physical sense 1) If you use a point load to do a plastic analysis, you will never get the converged solution. Because of the singularity at the node, on which the concentrated force is applied, the stress is infinite. The local singularity can destroy the whole system convergence behavior. The same thing holds for the contact analysis. If you simplify the geometry or use a too coarse mesh (with the consequence that the contact region is just a point contact instead of an area contact) you most likely will end up with some problems in convergence. point load plastic analysis contact analysis Geometry Mesh Suggestion

Suggestion : 

Suggestion KEYOPT(5)=1 KEYOPT(5)=0 FE Model is not modeled correctly in a numerical sense 2) A possible rigid body motion is quite often the reason which causes divergence in a contact analysis. This could be the result of the following: We always believe, that if we model the gap size as zero from geometry, it should also be zero in the FE model. But due to the mathematical approximation and discretization, it does not have necessarily to be zero anymore. Exactly, this can kill the convergence. If possible, use KEYOPT(5) to close the gap. You can also use KEYOPT(9)=1 to ignore 1% penetration, if it is modeled. One reason for convergence difficulties could be the following:

Suggestion : 

Suggestion Caution: If the gap physically exists, you should not use KEYOP(5)=1 to close it,instead, you should used the weak spring method. DELT=0.1 /prep7 et,1,183 et,2,169 et,3,172 mp,ex,1,2e5 pcir,1,2-DELT,-90,90 pcir,2,3,-90,90 rect,0,1,-7,-2.5 aadd,2,3 esiz,.3 ames,all Psprng,48,tran,1,0,0.5 lsel,s,,,1 nsll,s,1 Real,2 type,3 esurf lsel,s,,,7 nsll,s,1 type,2 Esurf R,2,,,,,,-1 /solu Nsel,s,loc,x,0 D,all,ux nsel,s,loc,y,-7 d,all,all Alls F,42,fy,0.11 Solv F,42,fy,2000 Solv Fdel,all,all F,48,fy,-.11 Solv F,48,fy,-3000 solv K=1, DELT=0.1 F=K*U To close the gap: F1=1*0.1+0.1=0.11 LS1: F1=0.11 LS2: F1=3000

Suggestion : 

Suggestion Numerically bad conditioned FE Model 4) ANSYS uses the penalty method as a basis to solve the contact problem and the convergence behavior largely depends on the penalty stiffness itself. A semi-default value for the penalty stiffness is used, which usually works fine for a bulky model, but might not be suitable for a bending dominated problem or a sliding problem. A sign for bad conditioning is that the convergence curve runs parallel to the the convergence norm. Choosing a smaller value for FKN always makes the problem easier to converge. If the analysis is not converging, because of the too much penetration, turn off the Lagrange multiplier. The result is usually not as bad as you would believe. FKN=1 FKN=0.01 One reason for convergence difficulties could be the following:

Suggestion : 

Suggestion One reason for convergence difficulties could be the following: FKN=0.01, KEY(10)=0 FKN=1: KEY(10)=0 Divergence FKN=0.01, KEY(10)=1 FKN=1: KEY(10)=1

Suggestion : 

Suggestion Quads instead of triads  Error in element formulation or element is turned inside out 6) If some elements are locally distorted you might get an error in the element formulation or the element is even turned inside out. Try to use a coarser mesh in this region to avoid those problems. You can also use NCNV,0 to continue the analysis and ignore those local problems if they do not effect the global equilibrium. In general, try to use triangular, tetrahedral or hexahedral elements (linear). Do not use quadratic hexahedral elements. Linear quads Mid-side triads Error in element formulation One reason for convergence difficulties could be the following:

Suggestion : 

Suggestion The parts have no unique minimum potential energy position. 7) If the max. DOF increment is not getting smaller and the force convergence norm keeps almost constant, probably some parts in the model are oscillating. Here, introducing a small friction coefficient is usually better than using a weak spring, not knowing exactly where to place it. Friction can be applied to all contact elements (try MU=0.01 or 0.1) MU=0.1 MU=0 One reason for convergence difficulties could be the following:

Suggestion : 

Suggestion Some times, if you define the contact and target properly, the analysis convergences much faster, and the result is also better. F

Suggestion : 

Suggestion Unreasonable defined plastic material 11) It is not always a good idea to define the tangential stiffness to be zero using a plastic material law. If the yield stress is reached all over the whole cross section, there is no material resistance anymore to carry the load. There will be a plastic hinge and so the solution will never converge. In this case, input the correct tangential stiffness. Plastic strain Stress strain curve with tangential slope zero One reason for convergence difficulties could be the following:

Suggestion : 

Suggestion Unreasonable defined plastic material Plastic strain Stress strain curve with tangential slope 10000 Stress distribution Contact region One reason for convergence difficulties could be the following:

Suggestion : 

Suggestion The fine mesh and similar mesh are always good for the contact simulation: Good mesh will generally make problem easier to converge. Geometry Sphere influence Mesh Normal stress Contact Pressure

Suggestion : 

Suggestion The fine mesh and similar are always good the contact simulation: Good mesh will generally make problem easier to converge. Geometry Contact mesh Contact region

Suggestion : 

Suggestion The fine mesh and similar are always good the contact simulation: Good mesh will generally make problem easier to converge. Normal stress Contact pressure

How can I make the problem converge? : 

How can I make the problem converge? Trust yourself: I’m able to make it converge! Consider the problem as idealized real world problem: 20%- Mechanics expertise, 20%- Engineer expertise 30%- FEA expertise, 30%- Software expertise Use the magic KEYOPTIONS