Hello:
I’m a post-doc at the University of Nottingham, and I’m using the hypoplastic model to simulate the centrifuge tests we did. The research area is related to soil-pile interaction. In the current model, we used the basic Coulomb friction law to simulate the soil-pile interface, but the results do not match well with the centrifuge tests. I think is because of the complex interface is not well simulated.

Does anyone know how to implement this Hypoplastic Interface Model into ABAQUS combined with the existing hypoplastic model subroutine?

For more information about our work:
https://www.researchgate.net/project/The-use-of-retaining-structures-to-protect-buildings-from-tunnelling-induced-damage

Thanks
Geyang Song

Tags:
8 Comments
  1. Hans Henning Stutz
    Hans Henning Stutz 6 months ago

    Dear Geyang Song,

    Do you look for a description of how to use it in CAE or an Input file?

    Best regards,
    Hans

    • Geyang Song Author
      Geyang Song 6 months ago

      Hi Hans:
      Thanks for your reply, yes, I’m currently using the hypoplastic model for my ABAQUS CAE, and the model parameters were calibrated.

      I think my question at the moment is not sure how to use this interface FRIC.

      In ABAQUS, Contact property: I think I need to set Tangential Behaviour-Friction formulation to User-defined. Then I don’t know what parameters I need to put in. Similar to the parameter used for the hypoplastic model?

      Is there any guidance that I can refer to?

      Thanks
      Geyang Song

  2. Arie Koot
    Arie Koot 6 months ago

    Dear Geyang,

    Can you not use thin layer elements with reduced soil parameters and tie this layer to the pile, instead of a contact?

    Arie

    • Geyang Song Author
      Geyang Song 6 months ago

      Hi Arie:
      Yes, it is possible, and I have tried it already. But the result did not perform well. Because in our centrifuge tests, the gravity is increased from 1g to 80g. Therefore, soil stress increased by 80 times. During this period, by using tie, ABAQUS is very difficult to converge. Our centrifuge tests also involve tunnelling induced ground movement, and I think using tie is not very realistic. I currently apply a friction coefficient (tan phi’), based on the triaxial test. This is because, for our centrifuge test, pile surface was bonded with sand, the same sand was used for centrifuge tests. So I just applied the basic interface model to the pile-soil interface. But during pile loading, most of the pile head load was transferred to the pile end, but for centrifuge tests, most of the load was transferred to the pile shaft. I believe this is because the current interface is not modelled correctly. So I want to try this hypoplastic interface model. But have difficulty in how to use it in ABAQUS.
      Thanks
      Geyang

  3. Le Chi Hung
    Le Chi Hung 6 months ago

    Hi Geyang,

    If you would attach your input Abaqus file here then we could help you easier.

    Chi

  4. Hans Henning Stutz
    Hans Henning Stutz 5 months ago

    Dear Geyang,

    basically in an input file the command would look like this:

    *Surface Interaction, name=IntProp-1
    *Friction, user, depvar=31, properties=26
    31., 1., 1e+06, 0.29, 0.61, 0.96, 1.09, 0.13
    2., 0., 0., 0., 0., 0., 0., 10.65
    0., 0., 0., 0., 0., 0., 0.72, 1.
    3., 1.

    Then you can use IntProp-1 in the contact definition, please don´t forget to define the normal contact as well. As a short explanation. Until property 23 it is the standard UMAT parameter, the properties 23= kappa_r; Props(24) = dsv; Props(25) = 3, Props(26)= 1

    where kappa_r is the roughness coefficient (see, e.g. https://soilmodels.com/download/stutz-h-masin-d-and-wuttke-f-2016-enhancement-of-a-hypoplastic-model-for-granular-soil-structure-interface-behaviour-acta-geotechnica-11-no-6-1249-1261-preprint/ )

    and dsv the virtual thickness coefficient (see, e.g. https://soilmodels.com/download/stutz-h-masin-d-sattari-a-and-wuttke-f-2017-a-general-approach-to-model-interfaces-using-existing-soil-constitutive-models-application-to-hypoplasticity-computers-and-geotechni/)

    Props(1)-Props(16) following the standard definition of the hypoplastic UMAT and Props (17)-Props(22) = 0, please also pay attention to the changed number of Props and state variables (statev). All of this definition have to be given into the contact properties tab in the CAE GUI in Abaqus.

    An additional side note is if you want to use the UMAT together with the FRIC – Umat subroutine you have to like both files for example in a user.for e.g.:

    include ‘Fric.for’
    include ‘UMAT.for’

    or copy both files together into one *.for file.

    I hope this descriptions helps you!
    Best regards,
    Hans

    • Geyang Song Author
      Geyang Song 5 months ago

      Hi Hans:
      Thanks for your help, this is very helpful !!!!!
      Best wishes,
      Geyang Song

    • Geyang Song Author
      Geyang Song 4 months ago

      Hi Hans:
      I recently tried to repeat your shear box test from the paper entitled ‘A general approach to model interfaces using existing soil constitutive models application to hypoplasticity’.

      I have successfully replicated the Mohr-Coulomb model (Figure 7 a, in the paper). (Mohr-Coulom interface, and Hypoplastic model for soil property)

      But I have a converge issue when using your interface model subroutine (Hypoplastic Interface Model, and Hypoplastic model for soil property).
      I followed your guidance and created a ‘user.for’ file, and included all the necessary model subroutine:

      include ‘umat.for’
      include ‘sdvini.for’
      include ‘FRIC_HPvW.for’

      Then I defined an interface property in ABAQUS:

      *Surface Interaction, name=IntProp-1
      1.,

      *Friction, user, depvar=31, properties=26
      31.4, 1e-08, 1968.63, 0.447, 0.624, 1.16, 1.392, 0.08
      1.5, 0., 0., 0., 0., 0., 0., 0.6926
      0., 0., 0., 0., 0., 0., 0.72, 1.
      3., 1.
      *Surface Behavior, pressure-overclosure=HARD

      Please note that my unit is in mm, and I think the parameter 16 (void ratio) from your previous reply input example should be 0.65 instead of 10.65.

      Then I run the simulation based on the following steps:
      (1) define an initial geostatic state (0.2 MPa along the depth of the soil )
      (2) Apply a vertical pressure of 0.2MPa at the top of the soil (I didn’t apply gravity and soil density)
      (3) shear the plate underneath the soil.

      By using your interface model, I can successfully run through step (2) (apply a vertical pressure). But ABAQUS won’t converge from step (3) at all. Not even a tiny time step.

      Do you have any suggestions? Did I miss some critical steps?

      Thanks
      Geyang

Leave a reply

©2020 SoilModels

Log in with your credentials

Forgot your details?