Learning Forum

[yasser1987]

Dear All 

 

i am trying to model a soil for single bucket foundation with  Mohr-coulomb failure criteria but unfortunately,when i define and insert the

properties of the soil i am faced with this error when i refresh the project to introduce materials and i cannot find the defined materials to assign the project 

 

here it is my model description for  Mohr-coulomb

 

 

i should mention when i delete the Mohr-coulomb from the project All the parameters goes well, i mean you can not get enough and precise solution even with warnings but at least works and this sign(red multiplication )will never show up 

 

 

for my project, i need to define the soil with Mohr-coulomb failure criteria but  actually, i do not know how to overcome these errors and problems 

please if someone has any idea or has already modeled a soil in ansys help me in this case 

 

 

Best regards 

Yasser

[jj77]

You just need to define the values in the yellow areas as you show in your image above. As I am using other software for soils, I am not sure what values, to enter there, but I am sure you can find out values for sand that you are using. Perhaps setting the residual values (cohesion, friction angle), to half of the initial one is a start.

 

I would also consider extending the outer boundaries (where it is fixed), so not to have any influence on the results. Also on the outer syl. surface I would put only radial fixed support, and at the bottom, only perpendicular (Y direction). To prevent rotation about one could fix a couple of vertices in the tangential direction so it does not spin about Y. 

[yasser1987]

many thanks for the response and suggestion 

 

but how can I define the radial fixed support !! since there is no option for the radial fixed support in the support section of ansys but  if you mean restricting the boundary with circle fixed  shape  i have already  made it I defined the boundary(circle shape) then select the fixed support, you can see my attached files and also how can i restrict the only Y direction at the bottom,

please help and guide me 

 

 

regards 

Yasser  

[jj77]

not sure, exactly how, but there is an option normal to a face, I think. In the mean time just try to run at as you have it.

[yasser1987]

Dear All 

 

 

i have found a paper that describes how to model a soil with mohr coulomb  and its Boundary condition, but i cannot understand how to apply this kind of boundary condition to my model in Ansys, i mean which options and icons must be used in order to apply the BC and etc

could you please help and guide me to apply the BC to my model?

 

 

 

 

Regards

[jj77]

If you have an answer to your original question, mark that post with Is Solution. Open a New Discussion for a new question, say related to boundary conditions in soil analysis.

[jj77]

Please post your question, and will try and reply. jj77

[Rana Nasser]

Hi Yasser,

Could you please add the link of the new discussion here (with your question)?

Best regards,

Rana

[yasser1987]

Here you are 

/forum/forums/topic/boundary-conditions-in-soil-analysis/?order=all#comment-f7205716-f0b0-4935-b9cc-a9d200a6c5e5

[shiv]

1) Modelling Mohr-Coulomb in ANSYS Mechanical Workbench

   There is a direct option for giving Mohr-Coulomb in ANSYS Workbench Mechanical from its 17 version. If you are using previous versions, then you need to define the Mohr-Coulomb using APDL macros into the mechanical model. Here below I have give a sample command snippet for defining Mohr-Coulomb inside ANSYS Mechanical Workbench..

/prep7

! ELASTIC CONSTANTS

MP,EX,1,20.0E9 

MP,NUXY,1,0.2

 

! Mohr Coulomb yield surface

         phi=30         ! friction angle 

         c=8.7e6        ! cohesion

         psi=15         ! dilatancy angle

         phir=20        ! residual friction angle

         cr=0.8*c       ! residual cohesion

         sigt=3e6       ! tensile strength

         sigtr=0.8*sigt ! residual tensile strength

 

TB,MC,1,,,BASE

TBDATA,1,phi,c,psi,phir,cr

TB,MC,1,,,RCUT

TBDATA,1,sigt,sigtr

TB,MC,1,,,RSC

 

TBDATA,1,0

 

Note: For better convergence use SOLID65 element(assume the model trying model is brittle in nature). And also keep check on the non-linear controls in the Analysis setting. Meshing should be Non-Linear and linear element.

 

2) Defining radial boundary condition. 

   You can use "Cylindrical support" boundary condition for directly define the radial support or you can use "Remote Displacement" for the defining the radial boundary condition. 

Note: For Soil modelling you can also use Drucker-Prager Piecewise model. 

 

Hope this clears your doubts regarding Mohr-Coulomb in ANSYS. In case of any other clarification feel free to comment back. Thanks