In the Sol 400 UG, chapter 13, it states “The current implementation is restricted to the requirement of a set of STATIC supports that constrains all six
rigid body motions only. Please note that the constraints must be only removing the rigid body motion, but not
induce any addition deformation and stress. Thus no mechanisms or symmetry boundaries are allowed.” I am not entirely sure how to create this condition. If I restrain a node it will induce stress at that point.
Is there a feature that will allow a nonlinear material analysis without any restraints? I was running the solution with inertia relief, but I had linear material properties. As soon as I introduce the nonlinear material the solution failed. I tried param,inrel,-2, but that didn’t work either.
Sincerely,
Christopher (Chris) J Wright
TEAMS 3 Engineer
Analytical Mechanics Associates, Inc.
NASA Langley Research Center
Hampton VA 23681
Office 757-864-2578
Mobile 801-866-9504 (Personal)
Christopher.j.wright-1@nasa.gov
This electronic message transmission contains information that may be proprietary, confidential or privileged. The information is intended solely for the recipient and use by any other party is not authorized. If you are not the intended recipient, be aware that any disclosure, copying, distribution or use of the contents of this transmission is prohibited. If you have received this electronic transmission in error, please notify the originator of the message.
The way I understand SOL400 works with inertia relief is you must add that case control command (IRLOAD=QLINEAR) and you can define a set of statically determinate constraints (and only statically determinate- just enough to remove all possible rigid body motion). These constraint DOF will become the reference DOF for the inertia relief solution.
Look at the Inertia Relief section in the Linear Static Analysis User Guide to see how to define appropriate 'SUPORT' DOF... these are the same rules you should follow when defining the 'constraints' for SOL400 with IRLOAD=QLINEAR turned on.
If you make a sample you can share, and you can't get it to work, please open a support case and mention my name and I'll help out.
Also, I have just done a test, and in v2019, and it looks like it worked fine... it is attached. Check out the SPCFORCE results to see that there aren't really any forces, so it isn't 'really' constrained.
