Model with nonlinear Contacts not converging due to (small) initial Rigid Body Motions in a Static Analysis (model underconstrained)
March 17, 2023 at 1:11 pmFAQParticipant
In Static Analyses of Assemblies with nonlinear contacts (frictionless, frictional, rough), it easily happens that not all parts of the model are initially in well-defined contact with their neighboring components. Then, initially, free rigid body motions are possible, which lead to a singular (or very close to singular) Stiffness Matrix such that the resulting equation system cannot be solved for a unique solution. Accordingly, convergence problems are met from the very beginning. A typical example for this situation is, when a gap in a bearing shall be taken into account. In these cases, it can be helpful to use the Quasi-Static solver option (TINTP,QUAS). As this option uses backward Euler time-integration, it is indeed not part of a real STATIC solution algorithm but of a TRANSIENT one. Accordingly, it requires switching to the analysis type transient and usually is more computationally expensive than a simple static analysis (with nonlinear contacts). ANSYS Help https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v190/ans_str/Hlp_G_STR5_12.html “For this option, the program uses backward Euler time-integration. The high numerical dissipation in this time-integration scheme can help to achieve convergence in some problems that are quasi-static in nature but fail to converge in a quasi-static analysis. … The automatic time incrementation does not try to maintain any minimum points per cycle, therefore allowing use of much larger time increments. … Applications that can benefit from using the QUAS option include: – buckling dominated simulations – models that may display temporary rigid body modes – and simulations that have a snap-through event, causing instability.” Nevertheless, in a ‘Static Structural’ Analysis in Mechanical, it can be invoked by just a small command snippet with very few APDL commands. Just insert a command snippet under the Static Structural branch ANTYPE,TRANS! switch to analysis type transient TINPT,QUAS ! switch to quasi-static solver option and make sure that you choose a small enough time step as initial time step size (e.g. 0.0001 s). Please also find a very simple example project attached, which contains a static and a transient analysis block. In each of them, the quasi-static solver option is invoked. Finally, please note that Contact Stabilization can be an alternative to the procedure described above. ANSYS Help https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v190/ans_ctec/Hlp_ctec_realkey.html Chapter 3.9.15
Introducing Ansys Electronics Desktop on Ansys Cloud
The Watch & Learn video article provides an overview of cloud computing from Electronics Desktop and details the product licenses and subscriptions to ANSYS Cloud Service that are...
How to Create a Reflector for a Center High-Mounted Stop Lamp (CHMSL)
This video article demonstrates how to create a reflector for a center high-mounted stop lamp. Optical Part design in Ansys SPEOS enables the design and validation of multiple...
Introducing the GEKO Turbulence Model in Ansys Fluent
The GEKO (GEneralized K-Omega) turbulence model offers a flexible, robust, general-purpose approach to RANS turbulence modeling. Introducing 2 videos: Part 1 provides background information on the model and a...
Postprocessing on Ansys EnSight
This video demonstrates exporting data from Fluent in EnSight Case Gold format, and it reviews the basic postprocessing capabilities of EnSight.
- ANSYS Mechanical: Fatigue Crack Growth Analysis using SMART Crack Growth
- Can the contact type (bonded or frictional) affect thermal results?
- How can I understand Beam Probe results?
- Which time integration scheme is used in transient thermal analysis and how to change the scheme?
- Modeling Radiative Heat Transfer
- Why there is difference in contact status between two load steps during Bolt Pretension? LS1: Bolt is Loaded LS2: Pretension is locked
- Static Structural Analysis of a Rear Upright – Part 1
- What is pinball radius and does mesh size effect this value?
- Stress Concentration Tips & Tricks
© 2023 Copyright ANSYS, Inc. All rights reserved.