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
Solved! Go to Solution.
Solved by John_Holtz. Go to 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,
A co-worker took a quick look at the model and made the following suggestions:
Let us know what you find out.
John
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
Can't find what you're looking for? Ask the community or share your knowledge.