Why do I get an error message, when trying to assess a crack? “One of the initial crack’s mesh or the crack propagation encompasses multiple bodies…”
January 25, 2023 at 7:34 amFAQParticipant
Such a Mechanical model for crack assessment often contains 3 error messages. 2 error messages in Mechanical “One of the initial crack’s mesh or the crack propagation encompasses multiple bodies which have more than two material models, which is not supported. Ensure one material model by scoping these bodies to one material assignment object and re-solve.” “An error occurred inside the SOLVER module: general error.” and 1 error message in the solver output “*** ERROR *** CP = 3.141 TIME= 12:24:07 Fracture parameter calculation issue: Contour integration for crack 1 has detected more than two material models in the domain integration, which is not supported. The contour integration results may not be correctly calculated.” The latter in Mechanical simply refers to the error message in the Solver Output. The other error message in Mechanical and the error message in the Solver Output both refer to the same thing: The APDL solver requires all elements over which the contour integral is evaluated to be assigned the same material ID. However, Mechanical by default assigns a proper material id to each body in the assembly, even when all of these bodies have been assigned the same material (in the details of the body objects). Consequently, the contour integral runs through elements with different material IDs. These error messages were introduced in release 2019R2 and only occur since then. Their purpose is to make even more clear to the user that contour integral evaluations (and associated theoretical considerations) may not apply to interface cracks or even multimaterial cracks. (SIFs calculation at any kind of multimaterial cracks is at least doubtful if not nonsensible from a fracture mechanics theory point of view.) How to overcome this issue? The first error message in Mechanical already tells you what to do: “Ensure one material model by scoping these bodies to one material assignment object and re-solve.” You can assign just one material ID to several bodies in Mechanical by following the following steps: – Select all bodies which are directly attached to the crack front/crack tip – Right Mouse Button click on the wanted Material under the Materials branch (in the Mechanical tree on the left) > Create Material Assignment Keywords: error, contour integral, J-Integral, Jint, Stress intensity factor, SIFs, T-Stress, tstress, crack
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.
- Question: What is the difference between PLNSOL, EPPL, EQV and PLNSOL,NL,EPEQ?
- ANSYS ACCS: Simulation of a Composite Rib Using ANSYS Composite Cure Simulation Tool
- ANSYS Mechanical: Delamination Analysis using Contact Debonding
- Is Johnson Cook model supported for static structural analysis?
- Hyperelastic Simulations
- How to use layered section to simulate composites and post process the results in ANSYS Mechanical
- Guidelines of modeling a gasket.
- Does it make sense to use viscoelastic material in static structural since it requires the calculation of strain rate?
- What are Isochronous stress-strain curves? How can they be used in ANSYS for modeling creep?
- When the material data sheet of a polymer reports both the Tensile and the Flexural Modulus, which value may be used in place of Young’s Modulus?