Nonlinear Transient Analysis > Problem with constraint motion (CBUSH, Hinge)

[kf065]

Hi,

I’m having trouble understanding the behavior of my Model.
The Setup consists of a hook, which rotates around a fixed pivot, and a solid recess.
The hinge, and the rigid connection is modeled with CBUSH elements,
and the force is applied as pressure on the top faces.
To archive the desired displacement, I used the “larger spring method”,
as the nltrans solution does not support enforced displacements.

I would expect this to result in circular motion, but I only get linear motion.
I’ve tried the following changes, but always get the same issue:

> Different element types: RBE2/RBAR/PBEAM/CBUSH(different stiffnesses)
> Position constraint with cylindrical coordinate system
> Different solver settings: LGDISP/LANGLE(1,2)/RTOLB/diff. stiffness update methods
> Run Model as static nonlinear solution.

Obviously, I’m missing something here, but after days of trial and error I simply can’t find the error.
This is starting to cause me sleepless nights - I would be happy if someone could help me out with this: )
I’m new to FEM and use AD Nastran for a university Project.

best regards
Kevin

[John_Holtz · Accepted solution]

Hi Kevin,

You may need to find someone who has access to FEMAP so that they can help decipher the model. I do not have any tools that will display the model, so I cannot confirm many details. For example,

1. How did you implement the large spring method? If you are trying to rotate the arm by X degrees, you would have a torsion spring with a large torsion resistance, then apply a moment to rotate the arm X degrees. (This article describes the equivalent for a large translation. https://help.autodesk.com/view/NINCAD/2022/ENU/?caas=caas/sfdcarticles/sfdcarticles/Nastran-In-CAD-E...) I am not sure how you are converting the pressure to a rotation or displacement since I cannot interrogate the springs.
2. I think node #5 (top left corner of the arm shown in your figures) is not moving purely in a linear direction. I calculated the changing Y and Z displacement for each output step (dY and dZ from previous step), and then calculated dZ/dY for each step. That should indicate what direction the node is moving on each step, as in tan(direction) = dZ/dY. The direction changed by approximately 0.8 degrees. Smaller than I would have expected since it looks like about a 5 degree rotation, but I don't know what the model is setup to do.
3. This is not related, but I noticed the convergence tolerance for displacements was changed from the default value (usually 0.0005) to 0.01. Such a large tolerance could allow the solution to drift. (Except that the load and work convergence tolerance appears to have "kept it on track". I think you got lucky.)

A co-worker took a quick look at the model and made the following suggestions:

1. Put all nodes (definition and output coordinate systems) into a consistent cylindrical coordinate system with the z-axis pointing in the axis of rotation. (There are 4 different systems used in the model; maybe there is a conflict or miscalculation that is causing the problem.)
2. Use stiff beams for the ‘rigid connections’.
3. Remove all contact and get the part rotating correctly first. If that works, then add contact.

Let us know what you find out.

John

[kf065]

Hi John,

fixed it – finally !

Many thanks for your and your co-workers feedback !

The Problem had to do with my use of the rigid elements. I was unaware that not all element types
support large nonlinear displacement. The RBE2 element operates only by small displacement theory,
which explains why I only got linear movement in my first Setup.

Solution:

PARAM,RIGIDELEM2ELAS,ON
PARAM,RIGIDELEMTYPE,BAR

Setting these two parameters manually fixed the displacement problem – alternatively, as pointed
out by your coworker, modeling the connection with stiff beams or solid elements (as mentioned in
the Femap Forum) also works.

I also noticed that the stiffness update method (Field 6+7 in TSTEPNL) had a huge impact on the
convergence of the model. Continuously updating the Stiffness Matrix every 5th or 2nd TStep
greatly improved contact stability, compared to the adaptive or automatic methods.
The model now also convergences with much higher displacement tolerances, which was an another
issue I had before - thus such a high tolerance, temporary fix ; )

The "larger-spring" method was implemented by attaching spring-to-ground elements to the end of the
hook and approximating the displacement force using hooks law.
This also simplified the model quite a bit (no CBUSH elements needed).

The Model seems to behave very well now – even for short duration “impact” scenarios and runs
surprisingly quick.

best regards
Kevin