Learning Forum

[Juanjo]

I am trying to solve a structural problem but solution doesn’t converge or some elements become distorted. Basically, a flat ended indenter punches a very soft material. I am using a Neo-Hookean hyperelastic model. 

Since there are too many variables to change in the indenter to get a converged solution, I am testing the basis of the problem with a very simplified model. This second model is a cylinder of Neo-Hookean hyperelastic material in which radius and height are equals. The model takes advantage of its axial symmetry to solve faster.

The lower circular base of the cylinder is fixed (Uy=0) and the upper circular base can be loaded in two alternative ways: either by displacing downwards the upper circular base; or by applying a pressure on it. 

When I set the model in “displace mode”, I can obtain easily a solution even compressing the cylinder an 80% of its height. For this displacement, the Y-component of stress allows to calculate the weight necessary to obtain the same displacement (1.637 Kg).

However, when I set the model in “weight mode” and load the upper tap with 1.637 Kg, solver terminates by “error in element formulation” or “unconverged solution”. I only get to compress the material a 28%.

The question is… WHY? Both problems (displace mode and weight mode) are the same in terms of element and material capacities, but the second fails. I think that my original and complex problem to which I referred to in the first paragraph fails because of the same reason that this simplified model. 

Thanks in advance!

The code is:

FINISH  
/CLEAR,START
/PREP7

!*****CONTROL PANEL: HERE YOU CAN CHANGE MODEL PARAMETERS.

!Geometry parameters:
   Height=0.01              !Cylinder Height (m)
   Radius=Height        !Cylinder Radius (m)
   NEle=10            !Number of elements at each lines of the model.

!Material model
   EX01=30000        !Young Modulus (this data is used later only to assess the equivalent Neo-Hookean model parameters)
   PRXY01=0.49        !Poisson's Ratio

!Load Parameters
   ByWeight=1        !If 1, a uniform weight is applied on the upper cylinder tap. If 0, a downward displacement is applied.
   Weight=1.637        !Weight in Kg. 
   Displac=-0.8        !If negative, downward displacement divided by cylinder Height.

!Time Control 
   Time_sim=1        !Simulation Time. Loads are ramped along the simulation time. 

!*****END OF THE CONTROL PANEL

!MATERIAL SECTION

nhmu01=EX01/2/(1+PRXY01)    !This is the "mu" parameter of the Neo-Hookean model
nhK01=EX01/3/(1-2*PRXY01)    !This is the "k" parameter of the Neo-Hookean model, Bulk modulus
nhd01=2/nhK01            !This is the "d" parameter of the Neo-Hookean model

TB,HYPE,1,1,2,NEO   
TBTEMP,0
TBDATA,,nhmu01,nhd01,,,,  

!***ELEMENT DEFINITION

ET,1,PLANE183   
!*  
KEYOPT,1,1,0        !Cuadrilateral element shape
KEYOPT,1,3,1        !Axisymmetric element behavior
KEYOPT,1,6,0        !Pure displacement for element formulation.

!****MODEL CONSTRUCTION

BLC4,0,0,Radius,Height,

!****MODEL MESHING

MSHAPE,0,2D 
MSHKEY,1
MAT,1

LESIZE,1,,,NEle,,,,
LESIZE,2,,,NEle,,,,
LESIZE,3,,,NEle,,,,
LESIZE,4,,,NEle,,,,
AMESH,1,,

!SETTING THE MECHANICAL CONSTRICTIONS
DL,1,,UY,0
DL,4,,UX,0

FINISH
/SOLU

ANTYPE,STATIC         !Static Analysis.
NLGEOM, ON        !Large Deformation

OUTRES,ALL,ALL,        !all data to inspect the solution

*IF,ByWeight,EQ,1,THEN
   SFL,3,PRES,9.8*Weight/(3.1415*Radius**2),
*ELSE
   DL,3,,UY,Displac*Height
*ENDIF

TIME,Time_Sim 
AUTOTS,1
DELTIM,Time_Sim/1000,,1
KBC,0            
SOLVE

[John Doyle]

Perhaps you need a lot more time increments.

Your "weight mode" approach appears to be a force based load (via SFL,,)

Your "displace mode" approach is a direct displacement (DL,,,).  The displacement approach is inherently more stable than the force based approach.

If you post process your force vs displacment reaction for the converged solution, that might give you some helpful feedback as to how much force the structure can handle before failing with element distortion error.

Also, try lower order elements (PLANE182) with enhanced strain (KEYO,,1,2) for more robustness.

[Juanjo]

Hi John, your help is greatly appreciated!

Yes: “weight mode” approach is a pressure load applied on the upper circular base of the cylinder: “SFL,3,PRES,9.8*Weight/(3.1415*Radius**2),”

And, again, the “displace mode” approach is a direct displacement as you have noticed.

I have tried to change a lot of parameters, but none of them improve significantly the results (NEle from 5 to 100; Time_sim from 0,1 to 10; automatic or manual step size…)

Yes, I also tried switching to PLANE182 but no big improvements: It allows us to compress the material up to 37% instead of 31%.

Yesterday I read something that worried me in the ANSYS manual (Explicit Dynamics Analysis Guide). In the section "7.6. Hyperelasticity", it says that

"The different models are generally applicable over different ranges of strain as illustrated in the table below, however these numbers are not definitive and users should verify the applicability of the model chosen prior to use" .

The range they give for the Neo-Hookean is 30%. Does this mean that an element whose material is Neo-Hokean cannot have a deformation greater than 30% of its dimension at rest? If so, this would explain everything, wouldn't it?

Thanks, John (and any else who help in this issue!)