March 17, 2023 at 8:59 amFAQParticipant
1) For polymers it can be difficult to separate the elastic strain from the plastic strain (as you would have to do to prepare the input curve for MAT_024 from a tensile test result) because the stress-vs-total strain curve at high strain values can be steeper than the initial elastic modulus. In those cases, it is easier to input the stress-vs-total strain curve as with MAT_089. 2) MAT_089â€™s ability to have failure strain as a function of strain rate is useful for polymers, some of which become more brittle at high strain rates. 3) Unlike MAT_024, the hardening slope of MAT_089 can be larger than the initial modulus. The unloading/reloading stiffness of MAT_089 is equal to the maximum tangent stiffness attained before the unloading occurs. On the other hand, MAT_024 unloads/reloads always with the initial modulus, therefore, the hardening slope in the MAT_024 should not exceed the initial modulus. 4) In years gone by, before *MAT_ADD_EROSION was added to the code, MAT_089â€™s basing failure on the maximum principal strain (rather than plastic strain) would have been a fourth point on the list. Additional information can be found in the remarks for *MAT_PLASTICITY_POLYMER in the LS-DYNA Manual Volume II.
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 LS-DYNA equivalent of *MODEL_CHANGE card (in ABAQUS). Which keywords can be used to introduce(activate)/delete(deactivate) elements in the middle of a calculation (at user-specific time/load steps).
- 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
- How to deal with “”Problem terminated — energy error too large””?”
- After Workbench crashes, how can I recover the project from a .mechdb file?
- How to display the color of each body based on the material in Mechanical?
- How to resolve “Error: Invalid Geometry”?
- Model has a large number of contacts – how to reduce them?
- Please explain the difference between Point Mass and Distributed Mass.
- How to locate an element of a particular ID number in Mechanical?