effecient contact simulation-compression only boundary condiyion? 1

[acrmnsm]

Hi we are trying to simulate a flange bolted down to a much stiffer plate, for conservative reasons we just want to set the boundary condition at the flange contact face. So rather than simulating the larger stiffer plate and the contact between that and the flange face, is there a way of simulating a compression only fixity?

In the past I have done this in other software using zero length or very short truss elements with a stress strain curve with very stiff compression and very soft tension. In other software there are options for either one way BC's, eg fixed in -ve U1 but free in +ve U1, or even a compression only BC.

Any advice as to how to achieve this in Abaqus CAE?

Thanks in advance

 

[burningDiesel]

"zero length or very short truss elements with a stress strain curve with very stiff compression and very soft tension"

Is a good way to do it I guess. Any reason why this didn't work? (or you didn't try yet?)
Another way is doing the same but with connectors, using non-linear elasticity.

Afaik, there is no easy boundary condition to do it.

 

[acrmnsm]

I haven't tried it yet because I was hoping there was a simple solution/am lazy.
In Ansys there is a compression only constraint, pic your surface/nodes/edge and click add constraint - pick compression only. Simple...
I have emailed our local support in the uk, if they don't have a simple/quick way of doing it then my olde skool method is going to be employed.

 

[corus]

Have a restrained rigid surface as the stiffer plate and just define contact, allowing for separation.

 

[acrmnsm]

I think this

Have a restrained rigid surface as the stiffer plate and just define contact, allowing for separation.

Is just a rephrasing of my OP :

So rather than simulating the larger stiffer plate and the contact between that and the flange face, is there a way of simulating a compression only fixity?

Or are you doing something different that I have missed?

This is the most obvious/easiest to set up, but my experience is that it is often better to develop as computationally efficient method. Contact problems often take longer to converge or have difficulty converging. My past use of zero length truss elements in some other fe software or Ansys compression only constraint seem to have positive effects on solution time.

 

[IceBreakerSours]

Very stiff compression and soft tension will result in a continuous but non-smooth stress-strain curve which will result in a jump in the tangent stiffness matrix thereby - potentially - making the convergence an issue, particularly if more nonlinearities are involved. A soft contact would do the same thing but without the limitation of the possibility of convergence issues as pointed out above. However, either way, the more nonlinearities you pile up, the more difficult time an implicit solver will have.

Are you new to this forum? If so, please read these FAQ:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[acrmnsm]

Well, only from 15 years experience, I have found that the stiff compression/soft tension method converges faster than using contact, unless you actually specify gap elements then this works well. I was specifically wondering if any one had used a compression only boundary condition, if none of you have any experience of a boundary condition like this then I think perhaps it does not exist in Abaqus.

 

[acrmnsm]

In fact on reading this again:

Very stiff compression and soft tension will result in a continuous but non-smooth stress-strain curve which will result in a jump in the tangent stiffness matrix thereby - potentially - making the convergence an issue, particularly if more nonlinearities are involved. A soft contact would do the same thing but without the limitation of the possibility of convergence issues as pointed out above. However, either way, the more nonlinearities you pile up, the more difficult time an implicit solver will have.

I think this is not quite right, as a contact model is also a discontinuity, it is essentially a stiff compression, zero tension stress train curve.
The reason my truss model converges so well is because the solver can predict at each step how much the truss will deform.

 

[IceBreakerSours]

The underlying assumption in my comments has been that 'contact' is of interest and more nonlinearities (large strain, large rotation, finite sliding friction contact, etc.) 'may' come into play at a later time as the modeling progresses. If none of this on the cards, then I am with you; yours is a clever approach. So, again, you may have it right but my understanding comes from the 'math' of contact formulation itself. With that in mind, let me clarify my opinion.

The reason, IMHO, for the high rate of convergence is because you are simply using a 2 node element assigned with linear properties in tension and compression, with the non-smooth character coming into play only when there is a transition. Likewise, gap contact elements, in reality, are non-linear springs, which explains your similar experience with gap elements. I am not sure if the documentation says so but I am quite sure that FEA developers do not recommend gap elements any longer (keeping in mind my assumptions).

The reason why 'contact' takes 'much' longer to converge is because the code has to identify the normals on the master surface. In fact, the space must first be discretized by 'invisible' elements. If the surface isn't smooth or if there is finite sliding or friction, the computational expense increases dramatically. In such a situation, if you add other nonlinearities, the solver *will* have a very hard time to converge to a solution. Indeed, you may even have to switch to Explicit.

However, if you have smooth flat surfaces opposing each other with little to no sliding and frictionless interaction, then the problem becomes *very* simple for the solver to solve.

Section 21.2.2 of the Analysis User's Manual (v6.11):

"Stability

Using no compression or no tension elasticity can make a model unstable: convergence difficulties may occur. Sometimes these difficulties can be overcome by overlaying each element that uses the no compression (or no tension) model with another element that uses a small value of Young's modulus (small in comparison with the Young's modulus of the element using modified elasticity). This technique creates a small “artificial” stiffness, which can stabilize the model."

This statement, I believe, explains our opinions/experience.

Now, coming to your point, yes, contact is a nonlinearity in itself but there are exponential (soft) contact models available in Abaqus that are 'smooth'. You can assign small parametrized tensile stiffness and an appropriate (chosen by the analyst) compressive stiffness.

Are you new to this forum? If so, please read these FAQ:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[acrmnsm]

If none of this on the cards, then I am with you

in my OP I said this:

flange bolted down to a much stiffer plate, for conservative reasons we just want to set the boundary condition at the flange contact face. So rather than simulating the larger stiffer plate and the contact between that and the flange face, is there a way of simulating a compression only fixity?

So in this case the contact of the flange is of interest, but only in terms of its reaction with the boundary condition - ie it is infinitely (or very) stiff.
Otherwise, I too would use contact...