Dividing geometries

[Clarabella]

This webinar could be useful for you:

#014 Links and Interactions between Nodes and Elements

The link to our webinars:
https://asdeasoft.net/?webinar

regards

[STKO Team]

Since I am trying to add a simple "stick" SDOF structure on top of my soil/foundation domain, I get the error that "Different NDOF at same node (node = 1, NDF1=3, DNF2 = 6)"

If you merge 2 geometries and assign 2 element properties with incompatible DOFs (in OpenSees) this is the error that pops up.
More specifically the common node between the beam and the soil would like to have NDF=3 from the soil element, and NDF=6 from the beam.
What you need to do is to keep the beam and soil geometries separated. Then you can link them with an interaction. Finally, you can assign a Boundary COndition to this interaction.
The simplest EqualDOF(1,2,3) will solve the compatibility issue, but in your specific case, it will lead to a rotational release at them bottom of the beam.

You can use the Beam-to-Solid-Coupling interaction that we have in STKO. Ultimately, it is a mix of EqualDOF and RigidLinks to solve both the issue of different DOFs and the transfer of moment from soil to beam.
At minute about minute 22 of webinar #14 you can see how it works.

Keep in mind (and we also explain this isse in the webinar), that since there is a mix of multiple multi-point constraints, you MUST use the Penalty COnstraint Handler for the beam-tosolid-coupling

coupling.png (662.47 KiB) Viewed 3714 times

[kolozvari]

Thank you for your reply. I have applied the beam-to-solid coupling to my model that has a soil domain, a big foundation block, and a stick (beam) element with a point mass on top (see figure below).

Originally, I didnt see your latest message, so I used Transformation DOF numbered, and the model was able to successfully complete the analysis, but results didn't make sense because the foundation block and the stick didn't move at all even though the soil was shaking. I am guessing this is related to the fact that you cannot use Transformation method. Can you please confirm?

After seeing your message, I changed to the Penalty DOF numberer, but the model fails even for gravity loading.

Can you please take a look at the model (attached) and let me know if I assigned the beam-to-solid interaction correctly? Also, what should I do to try to improve the convergence? How do you choose parameters of the Penalty method? Please note that model of the soil converged just fine, as well as the model of the soil and beam with Transformation DOF numberer (clearly wrong thing to use, but it converged), so the issue must be related to the beam-to-solid interaction and the parameters of the Penalty method.

Thank you very much!

[STKO Team]

so I used Transformation DOF numbered, and the model was able to successfully complete the analysis, but results didn't make sense because the foundation block and the stick didn't move at all even though the soil was shaking. I am guessing this is related to the fact that you cannot use Transformation method. Can you please confirm?

I'm sure it was related to the Transformation method. A limitation in the Transformation method is that, if a node is a slave in a constraint, it cannot be a master or a slave in another constraint. The beam-to-solid coupling has this issue. The auxiliary node, is coupled with an EDOF to the soil, and with a RigidLink to the Beam.
In this case the Penalty is the only one that can handle this complicated configurations.

Before checking the model, let's review some rules that may create the issues you are experiencing:

• With the Penalty handler, NEVER use the NormUnbalanceTest! The norm unbalance will contain the reactions of the MultiPoint Constraint Penalty elements, and so it will never go to zero! Use the NormDispIncr instead.
• With the Penalty handler, choose a proper penalty parameter (it can be the same for the 2 penalty parameters).
  It should be large enough to impose the constraint, but not too large otherwise all other numbers will be seen as 0, and so the matrix will be numerically singular.
  You can evaluate it like this:
  • evaluate the typical stiffness entry in your matrix (no need to be precise). For a solid model it can be:
    K = E*Lch (E = soil young's modulus, Lch = characteristic length of your Finite ELement)
  • compute its Order Of Magnitude:
    oom = round(log10(K))
  • compute the exponent of the penalty parameter as
    ex = oom + 8 (why + 8? double precision floating point numbers have 16 significant digits. choosing 8 means "50% accuracy of the constraint, 50% accuracy of the matrix..."
  • here's the penalty parameter:
    p = 10^ex

Let us know if these rules can fix your issue

[kolozvari]

That worked! Thank you very much!

[HC2020]

Dear Kolozvari,
On Thursday, Massimo Petracca will be hosting a round table for STKO users and those interested in the field. If you are interested, we would be really excited for you to participate.
You can sign up here: https://asdeasoft.net/?stkowebinars-for-opensees

[hawrebelo]

you are doing a great job