Tagged: ls-dyna, LS-DYNA Suite, lsdyna, R13.x, structural-mechanics
March 17, 2023 at 8:59 amFAQParticipant
The accuracy of an implicit analysis depends on the convergence tolerances specified in *CONTROL_IMPLICIT_SOLUTION. The ultimate way to judge if your converged solution is accurate enough is to rerun the model with the DCTOL or/and ECTOL reduced by let’s say a factor of 10 and then compare the history of a critical response quantity to the history that was obtained with the larger tolerances. If the results are similar, it means that your original tolerances were likely good enough. If the results are different, it means that you need to lower the tolerances further. In other words, you need to see how sensitive your analysis results are to tighter tolerances. Note that it is recommended that RCTOL=1e10 and ABSTOL=1e-20 in *CONTROL_IMPLICIT_SOLUTION. The iteration data is written in the d3hsp and message files. Setting NLPRINT=3 in *CONTROL_IMPLICIT_SOLUTION will write the iteration data in greater detail, as described in the manual. The d3hsp can be loaded to LS-PrePost to visualize the implicit convergence statistics by selecting Misc>D3hsp View>Load>(pick d3hsp file)>Implicit Statistics. This allows, for example, for the user to plot the number of iterations required per time step, or the residual force norm, as well as the displacement and energy norms, at convergence per time step, or the norm values with respect to the iterations in a single time step. Visualizing the iteration data can help the user judge and adjust the convergence tolerances specified in *CONTROL_IMPLICIT_SOLUTION. For example, if an analysis takes too little iterations (like 2 or 3) to converge, it can indicate that there is room to lower the tolerances. Or, if the analysis takes too many iterations to converge for a given tolerance, it may show that the settings of *CONTROL_IMPLICIT_AUTO need to be adjusted or that the tolerances are too low. Furthermore, the absolute residual should be orders of magnitude lower than the applied load in your model. In addition, there is also the option to write the residual forces and other quantities to the binary database d3iter at every iteration of each output step. Fringing the residual forces may help identify in which areas of the model the convergence is weaker. This output is activated by setting D3ITCTL>1 in *CONTROL_IMPLICIT_SOLUTION and RESPLT=1 in *DATABASE_EXTENT_BINARY. The implicit solver will then write the d3iter database that is similar to d3plot. After the d3iter file is loaded into LS-PrePost (through File > Open > LS-DYNA Binary Plot > select the d3iter), the residual forces can be fringed through Post>FriComp>Ndv>Resultant Residual Forces.
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.
- The warning message is: “The maximum contact stiffness is too big. This may affect the accuracy of the results.” Why does large contact stiffness affect results accuracy?
- Contact Definitions in ANSYS Workbench Mechanical
- After Workbench crashes, how can I recover the project from a .mechdb file?
- Model has a large number of contacts – how to reduce them?
- How to resolve “Error: Invalid Geometry”?
- How to display the color of each body based on the material in Mechanical?
- Please explain the warning message “coefficient ratio exceeds 10e8” ?
- How to locate an element of a particular ID number in Mechanical?
- How to Connect Excel to Workbench
- How can I plot bodies colored by material property in Workbench?
© 2023 Copyright ANSYS, Inc. All rights reserved.