Search
Close this search box.
Notifications
Clear all

Drucker-Prager convergence problem

5 Posts
3 Users
0 Reactions
1,468 Views
Posts: 3
Topic starter
(@arul britto)
New Member
Joined: 15 years ago

Hi all,

I am very sorry, if I bother with a too simple problem, but: I try to simulate behavior of a dental composite (polymer resin- spherical particles) , using ABAQUS CAE. For resin with asymmetric yield stresses I use Drucker-Prager plasticity model.

If I run the material model with a unit cube of resin, it converges very quickly, even by introducing of high value of uniaxial displacement load (up to 6% of strain).

But if used for 3D simulation, it refuses to converge. I have tried many techniques of improve convergence, including mesh refinement, analysis step refinement, using other elements, but everything increased only the computational time and did not help with the convergence.

I try to model the shrinkage process of dental composite, obtain the residual stresses, then apply far-field load and investigate, how the residual stresses influence the mechanical response. Shrinkage of the polymer resin is up to 7%, so it is far in the plastic region of the resins stress-strain curve. Shrinkage is modeled by thermal analogy, this means, defining expansion coefficient &#945,, and decreasing temperature in model.

For the reason of computational time I use linear tetrahedron elements, but even use of other elements does not help with the convergence. For the Drucker-Prager model I use the linear shear criterion, deffault Flow Potential Eccentricity Friction and Dilatation Angle both of 28&#730,, Flow Stress Ratio 1 and tension-based hardening described by following stress plastic strain points

20 0

25 0.001

30 0.0014

35 0.0024

40 0.0033

45 0.0047

50 0.0076

55 0.0118

58 0.025

This describes the stress-strain curve well, even in plastic region, but only for uniaxial test-model of pure resin. By introducing three-dimensionality, even by a model of composite of 1 particle in block of resin and only shrinkage load, it needs more than 30 iterations, as the level of shrinkage reaches plastic value. Changing of the parameters of analysis step does not help.

In the stepmodule, I currently use static-general, Nl geom ON, increment size initial 0.1 , min 1E-005, max 0.2.

Please, would anyone of you be able to give me any suggestion or advice, how to improve the model to reach convergence, without significant increase of the simulation time? It will help me a lot with a a problem which I cannot solve for a long time!

Very many thanks,

Ondrej

Topic Tags
4 Replies
Posts: 3998
(@jorgen)
Member
Joined: 5 years ago

Have you tried to run your model with another simpler material model. Say an istropic hardening plasticity model (*Elastic, *Plastic), or even a simple hyperelastic material model.

My guess is that your material model may not be stable.

-Jorgen

Topic Tags
4 Replies
Posts: 3
Topic starter
(@arul britto)
New Member
Joined: 15 years ago

Yes, I have tried it. I run it with a von Mises material model, and this runs well.
I try to discover the reason of difficulties by a simulation of a unit cube of polymer resin, and as expected, it does not converge, if a quasi-hydrostatic tensile displacement BCs are prescribed (6% in each direction). If I use the same value in compression, there seems not to be a problem.

I was thinking about a hyperelastic model, instead of Drucker-Prager, but I am not sure, if it will match the physical reality in the material in a correct manner.

Is there any way to make the Dr.-Pr. model stable?

Many thanks,

Ondrej

Reply
Posts: 22
(@stusapien)
Eminent Member
Joined: 14 years ago

The loading that you apply (whether the tensile displacement or the thermal shrinkage) will result in a negative (tensile) p value and a zero deviatoric stress (q). That puts you on the negative horizontal axis in the p-q space (see documentation of Drucker-Prager material). Since the load magnitude is quite large, the material goes into plasticity as you mentioned. The flow rule will lead you to the apex of the yield surface (where it meets the horizontal axis). It may well be that the program has difficulty in converging at that highly nonlinear point. Still, in my opinion, convergence should be achievable. That would also explain why there is no problem when you load the material in compression. The uniform compression results in a stress state on the positive axis in p-q space (p>0, q=0) and in that case the material is always elastic and hence converges without difficulty. Also the von Mises plasticity does not have this difficulty.

I find it tempting to use the Drucker-Prager, or Mohr-Coulomb, plasticity models when the material has a yield stress that is different in tension and compression but they come with added complexity and stability issues, as well as non-symmetry of the stiffness matrix (may result even if you use the same friction and dilation angles).

Reply
Posts: 3
Topic starter
(@arul britto)
New Member
Joined: 15 years ago

Dear FEguru, many thanks for the reply. I think, you are right in all points. I have allready reached the convergence. It needed 14000 increments in the step, where the 7% shrinkage had been prescribed. But many thanks for the theoretical insight!

Reply
Share: