User login


You are here

Unconverged Mohr-Coulomb Plasticity, ABAQUS

Dear Abaqus Users,First of all, I want to clarify that I am a beginner in Abaqus (only few months) and new in iMechanica. I have been modeling an excavation in Abaqus/CAE. I am using several layers of soils which have been modeled using Mohr-Coulomb model, the wall as an elastic material. Both the wall and the soils were modeled with 2D solid elements (plane strain).I have been facing with lots of problem with the interaction of the first layer and the wall, "UNCONVERGED MOHR-COULOMB PLASTICITY" in the GEOSTATIC STEP!!!!. The first layer does not have cohesion, only friction which is 30 degrees (sand). After increasing the cohesion value for this layer, I can avoid this ERROR. But, lamentably, I am changing the whole problem with high values of cohesion which are around 30 kPa. The same effect can be reached using a surcharge which does not exist. Do you have any recommendation of how to solve this problem without changing the material properties?  Thank you very much!!!


PS: This is the problem I can see in Job Diagnostics... (image attached)




Donald X. Chen's picture

Scientific Computing and computing Scientifically.


Excavation is a typical problem of geotechnical engineering. I didn't use Abaqus to carry out the FE analysis of thus problems. But I did some with other softwares.  It seems that you are using the associated plastic flow rule (i.e. friction angle = dilation angle).

If unloaded Mohr-Coloumb soil with zero cohesion subjects to tension, the  convergence  problem may occure.


Good Luck!


X. Chen 


Hi Gonzalo

Same as Chen I think you are using the associated plastic flow rule. To avoid the problem use the option UNSYMM in your input file:


Hopefully it will solve your problem. 

Kazem Ghabraie

PhD candidate, Civil Engineering
RMIT University, Melbourne, Australia

Hi Kazem,

Could you also explain why using an unassociated flow rule will lead to convergence?  How do you choose the appropriate flow rule?

Also, I couldn't figure out whether the failure to converge was in the inner Newton iterations (at the Gauss points) or the outer Newton iterations (at the stiffness matrix level).  Could you clarify? 

-- Biswajit 

Donald X. Chen's picture


  What kind of plastic flow rule to choose depends on what kind of soil you are simulating.

F or the soil with dilation property such as dense sand, you may need the non-associated plastic flow rule.

PA VERMEER - Physics of Dry Granular Media, 1998

Usually, for non-assocciated flastic flow soil, you need non-symmetric linear solver which is embedded in the nonlinear algorithm

such as the Newton-raphson method. Based on my expeirence, for non-asscoaited plastic flow soil model,

the convergence for the nonlinear iteration method is more difficult, and it may also happen for iterative linear solver.

of course, it is due to that the out-of-balance error is more difficult to reduce. You may try to 

increase the number of load increments. 

For the stress point algorithm, we may usually  use the sub-stepping algorithm (see Sloan's paper)!



X. Chen 

Hi Donald,

My question more about the "why" than the "how" of nonassociated flow rules.  To paraphrase my earlier comment, I wanted to know why:

1) using a nonassociated flow rule will give better convergence than an associated flow rule (for a material will zero cohesion).

2) the yield surface is usually determined from experimental data.  How is the corresponding flow potential for a non-associated flow rule determined?  A brief explanation will be great.  (I'm too lazy to read a book on the subject :) 

-- Biswajit 

Donald X. Chen's picture

Hi, Biswajit

  (1) The first question is too difficult to answer because a lot of factors may influence the convergence, epspecially for a zero cohesion case. Thus, in many geotechnical softwares, it is recommended to use a small value  instead of a zero cohesion. In my previous studies, I found the convergence with non-assocated plastic flow should be more difficult.

  (2) The non-assocaited plastic flow rule is so called due to the difference between the Yield function and the plastic potential function. In Mohr-coloumb soil model, it is due to the difference between the friction angle and dilation angle. Because the topic is related to the Mohr-Coloumb model, we may only focus on it. In practical geotechnical projects, the two angles are both provided by experimental data.

While if we don't have such input, we may assume one based on: Normally consolidation clay soil may show little dilation, so we may assume \psi \approx 0. For quartz sands, we may use \psi \approx \phi -30. For soils with \phi < 30, we may use a zero or very small dilation angle.  (This comment is based on Plaxis material model manual, \phi is friction angle, \psi is the dilation angle).


Hope it is useful to you!


Donald X. Chen 


Hi Donald,

Thanks for the tips.

My own feeling is that non-uniqueness of the flow direction at/close to the tension tip may be  the reason that convergence is not achieved with asociated Mohr-Coulomb plasticity (with zero cohesion).  A non-associated flow rule often uses a potential that does not have a sharp tip and thus avoids the non-uniqueness issue.  What do you think?

-- Biswajit 

Donald X. Chen's picture

Yes, Now I undrstand why you emphasize the point of zero cohesion. Your analyse is reasonable, but I am not sure about your comment "A non-associated flow rule often uses a potential that does not have a sharp tip".

 It seems that for singular corners or the singular tip, special techniques have to be used to smooth the surfaces. 

Thanks also for your valuable comments!



Donald X. Chen 


 I believe that the convergence issue is due to one, or both of the following reasons:

 1. The use of zero cohesion implies that the soil cannot take tension - if there is tension in any of the elements in the mesh, one will encounter this problem of nonconvergence.  If one has a small cohesion value, the maximum allowable tension in the soil can be estimated by projecting the yield surface back intercepting the hydrostatic axis.  Note that ABAQUS does a default smoothing on the yield surface on the tension (negative pressure) side.  

2.  The use of dilation angle different that the friction angle implies the use of non-associative flow rule which leads to unsymmetric matrices.  One will need to invoke the unsymmetric solver to avoid convergence problems.  Incidentally, ABAQUS does a default smoothing of the corners of the multi-surface Mohr-Coulomb model.

Usually, I would use a small amount of stabilization (STABILIZE) to overcome the convergence issues associated with soil with zero or a very small cohesion value.  This allows dissipation of energy due to unstable response in the soil e.g. tension in soil, and therefore improves convergence.  However, one needs to verify that the stabilization will not affect the response drastically, because invoking stabilization is like using a "hand" to hold your soil to prevent failure (one should check that the energy dissipated by viscous damping is small when compared with the total strain energy). 

The other way to control convergence is to copy and overlay the same set of elements over the original elements and merging the nodes. The overlay elements are set to have elastic properties having a small Young's modulus - in this way, one can do without stabilization by using a small Young's modulus.  I would prefer to use the latter approach, but requires more work during the meshing stage.

I suggest that one does a one element test under load control in tension to see what I mean about Point 1. 

Hope this helps.


Dear All

I am a new user of ABAQUS. Can any body tell me how to define a soil with a linear changing Young's modulus with depth in ABAQUS?

Thanks a lot


Hello all,

I'm also a newbie in this soil modelling business; have modelled a 'tank' full of soil using C3D8I elements (hexahedral). A rigid pipe is located buried within the the center and imposed a translation. The model converges if I leave the material card alone and merely input the elastic properties. But once I input the *Mohr Coulomb model by inputting the friction angle and dilation, as well as the hardening card (cohesion 2.5kPa), the model refuses to converge. Basically using numbers provided so I'm unaware of how accurate they are.

The bricks do not even get squashed and instead, the analysis terminates as soon the brick gets compressed.

Anyone can help?

pls help me.. to vary friction angle with plastic strain in abaqus following mohr coulomb model


pls help me.. to vary friction angle with plastic strain in abaqus following mohr coulomb model


Frank Richter's picture

Subscribe to Comments for "Unconverged Mohr-Coulomb Plasticity, ABAQUS"

Recent comments

More comments


Subscribe to Syndicate