Contact modeling theory

[Anonymous]

Hi everyone!

I am quite new to Inventor and would like to ask something about how are contacts modeled.

I know that Inventor only performs linear analysis and was wondiring how certain contacts, such the separation-no sliding or the sliding-no separation contacts are modeled. With this type of contacts, in fact, the contacting area between the parts will change and geomertical non-linearitires will appear; in "conventional" FEM the load vector and possibly the stiffness matrix should be updated requiring a non-linear model for the solution.

Are linear springs set between contacting nodes used in Inventor instead? Or what is the trick?

I did not find a lot of theory on the Inventor guides I have consulted so far and was thinking maybe asking here would help.

Regards,

Jacopo

[raviburla]

Hi,

Thanks for the query. As you have noticed, Inventor Stress Analysis supports separation contacts and their variants. These types of contacts naturally lead to a non-linear problem. However, do note that the material modeling is still linear and small deformations are still assumed.

For the contacts modeling, the mesher/solver computes the contact entities automatically (note that this is not same as detect auto contacts). The contact entities form a set of triangles from one face and a set of triangles from a second face. Relations are developed between the contacting triangle-nodes based on the specific contact type. The formulation Augumented Lagrangian with inequality constraints. The system of equations (non-linear) are solved iteratively until equilibrium conditions are satisfied.  

Thanks,

Ravi Burla

[Anonymous]

Hi Ravi,

I agree with you that the material model is in this case still linear; but I do not beilive that small deformations can still be assumed in this case since due to the contact pressure the contacting areas will increase and therefore the solution will be geometrically non-linear (large displacements).

You say that the system will require a non-linear iterative solution but that small displacement are still applicable; arent the two statements in contrast? If the material is linear (and it is) and displacement are small why would we need a non-linear solution?

Moreover, from the manual of the software, this feature (non-linearity due to large displacement) is specifically excluded. This is why I think that the contact in Inventor are simulated using some other different approach than the classic non-linear solution adopted in FEM.

Best,

Jacopo

[raviburla]

Hi Jacopo,

The problem becomes non-linear even with small deformations because, the contacting condition could be ON or OFF for each contacting node. We will not be able to know the exact final condition for each node, unless we perform nonlinear iterations. For example, lets assume that two contacting surfaces are separated by small distance initially and the loading on the model is such that at equilibrium some nodes on the faces will be in contact and some others are separated. This equilbrium condition cannot be determined by just one linear solve. The non-linear iterations will stop once the equilbrium is attained - meaning that the "contact state"  of each node does not change with subsequent iterations. 

Please note that when bonded or spring contacts are used - no non-linear iterations are required. But when separation and its variations are used, non-linear iterations would be needed. 

Hope this clarifies your questions.

Thanks,

Ravi Burla 

[Anonymous]

Hi Ravi,

You are totally right. We would not need non-linear solution also if small displacement are applied. I wrongly formulated my question. But unfortunately I still have some questions marks in my understanding.

Basically my doubts are due to the fact that the Autodesk Inventor 2015 Guide says: 

"Stress analysis assumptions

Issue:

Stress analysis is used to solve linear, static problems. Although many engineering components fall into this problem category, there may be situations where the linear, static analysis assumptions do not apply."

This and the fact that I did not find any way to control the actual non-linear convergence, hence method or time-steps anywere in the software.

I would like to know which method and assumptions are used in the software (like for example compared to Ansys or Autodesk Simulation) since knowing this is foundamental for the interpretation and judgment of the result reliability and limitations. You cited "augmented lagrange method" as a contact constraint method. What is the iteration method instead? What are the timesteps? What are the limitations?

Best,

Jacopo.

[raviburla · Accepted solution]

Hi Jacopo,

Inventor Stress Analysis uses a hierarchical Finite elements for solution purposes and as the guide says - the solutions are limited to linear small deformation analysis only. However, when contacts are involved, some contact types lead to non-linear equations. I will try to explain it below:

Contact conditions can be represented in general as [C]{x} >= {d}. Here [C ] is a coefficient matrix, {x} is a vector of degrees of freedom which are involved in the contact, {d} is a vector which can be thought of as "separation distance". When the contacts are bonded/spring, then the contact conditions will degenerate to equality constraint:   [C]{x} = {d}. When using augmented Lagrange formulation, the equations will become of the form [ K + a*trans(C)*C,  trans(C) ; C, 0] {u, lambda} = {F, d}. This is a linear equation and can be solved in one solution-step.

However, when the contacting condition leads to inequality constraint: [C]{x} >= {d}, then the system of equations become: [ K + a*trans(C)*C,  trans(C) ] {u, lambda} = {F} and [C, 0] {u, lambda} >= {d}. These equations naturally form nonlinear system due to the presence of the inequality. Inequality conditions represent separation-type contacts. This is solved iteratively by setting the inequality constraint as equality with "active set of constraints". The equations are solved by updating the "active set of constraints" until the active set of constraints is stable (meaning that it has converged).

Since, the above is a very special treatment for contacts and is not the "classical non-linear solve with load increments", there is no control available for the user to define the time step information and such.

Hope this answers your questions.

Thanks,

Ravi Burla

[Anonymous]

Thanks Ravi!