Materials

Materials

Topics relate to Granta Design and more

    • Gaby Saad
      Subscriber

      Hello,

      I am trying to simulate Cam Clay in Ansys but the run is failing. First I drew my soil profile (having Shell181 linear element) as well as my foundation (having Solid185 linear element). Then I assigned the properties of Cam Clay (with density) to the soil and concrete to my foundation. Both the soil nd the foundation are shared to ensure that there will be no sliding or sepearation between the soil and the foundation. I established a structured mesh by partioning the soil in several blocks and created 2 step. In the first step, I established a varying stress profile (by applying an instantanous gravity to the model and using the function based command INISTATE) to the whole model. In Step 2, I applied the loads on the foundation in step 2. I also set up my boundary conditions to the model by having a fixity (Ux=Uy=Uz=0) at the bottom of the soil and rollers on the side of the soil layer. After finising all these steps, I run the model but it is failing and giving me the following error: 

      The material solution failed for element 108542 with material 6

      Can anyone help me with this issue? Your help is greatly appreciated. Thank you

    • John Doyle
      Ansys Employee

      How did you validate your material properties? Can you get a simpler 4 element test model to converge, without any other types of elements present (i.e. shells and contacts).  Can you get the same simple test model to produce same error message under tension and/or shear loading?  Is the element being called out in the error message going into tension perhaps?

    • Gaby Saad
      Subscriber

       

       

      I used the material parameter values of page 165 of the book of Potts and Zdravkovic, to simulate what is shown in Fig. 1 (below) for validation purposes:

      -          κ=0.025

      -          v=0.25 

      -          ah0=200/2=100kPa

      -          e0=v1=2.67-1=1.67

      -          λ_f=0.181

      -          Mc=0.797

      -          Initial stress state -200.1kPa, -200.1kPa, -200.1kPa 

      (inis,set,dtyp,stre
      inis,defi,all,,,,-200100,-200100,-200100,0,0,0)

      -          Ks=0.78

      using prescribed nodal displacements:

       

      and the resulting deviatoric vs axial strain graph turned out the same:

      I tried simulating cam clay with a simple 4 element test model to see if the solution will converge (having only solid185 element) with instate command and it did not work, the error still appears:

       The material solution failed for element “x” with material “x”

      (NOTE: the inistate command applied to my model is:

      inis,set,data,func
      inis,set,dtyp,stre
      inis,defi,all,,,,LINY,0,-17651.97,0,-17651.97,0,-17651.97,0,0,0,0,0,0                                                                                                                                                                                                                       The soil density is 1800 kg/m3 and the gravity is applied in step 1 at time 0 and 1s is 9.80665 m2/s)

       Any suggestions on why this error is appearing? Your help is appreciated.

       

       

    • John Doyle
      Ansys Employee

      It seems that the code cannot sort out where the stress state is on the yeild surface. 

      You might have seen this already, but if not, there is a Camclay example input script documented in Section 4.11 of the R2023-R2 Material Reference Guide.  That example will solve successfully with sample properties given for a 2D plane stress, (PLANE182) under a similar displacment load.    Can you start with that example and substitute your material data in for comparison?  

      I assume that all your material inputs are in consistent N-Meter (Pa) units?  You mentioned that aho=100kPa, but your INIST, appears to be in Pa.  Not sure if that might be part of the issue.

    • Gaby Saad
      Subscriber

       

      Hello, 

      It seems that the stresses were in tension rather in compression. I have simulated a model (only soil with solid185 element) having 4 elements and applied gravity as well as inistate command as shown below, but the problem is the initial stresses are not being applied linearly with depth. I am trying to establish a geostatic stress field such as σxx=σzz= K0*σyy where K0=1.

      Inistate Command:

      inis,set,data,func
      inis,set,dtyp,stre
      inis,defi,all,,,,LINY,0,17651.97,0,17651.97,0,17651.97,0,0,0,0,0,0

       

Viewing 4 reply threads
  • The topic ‘Cam Clay’ is closed to new replies.