What is the result item TENE? How is it defined, what is its physical significance, and how is it related to Joule heating in a SOLID69 thermoelectric model?
March 17, 2023 at 8:59 amFAQParticipant
The best way to determine how TENE is calculated and therefore what it represents physically is to create a test model using SOLID69. In the attached input file, APDL was used in POST1 to determine alternate ways of calculating both JHEAT and TENE. JHEAT is relatively straightforward. It is the ohmic heating per unit volume (W/m^3): JHEAT = J^2 * rho where J = calculated current density (A/m^2) Rho = electric resistivity (ohm-m) It appears that TENE follows the calculation of mechanical strain energy (element table item SENE). SENE is calculated as one half of the product of stress, strain, and element volume to give the stored elastic energy in each element (in Joules, not in Joules/m^3): SENE = 0.5*stress*strain*volume Following this logic, TENE should be equal to one-half the product of thermal flux, thermal gradient, and element volume. This can be thought of in terms of “across” (or “direct”) results data (displacement for structural, temperature for thermal), and “through” (or derived or reaction) results data (force for structural, heat for thermal). The analogous quantities for evaluating these energies are then: ACROSS RESULTS DATA Structural: displacement U => strain Thermal: temperature TEMP => thermal gradient TG THROUGH RESULTS DATA Structural: force F => stress Thermal: heat => thermal flux TF In the attached input file, TENE is read in and called TENE_1. APDL is then used to perform an alternate calculation of TENE that was called TENE_2: TENE_2 = 0.5*TF*TG*volume It can be seen that contours of TENE_1 and TENE_2 are almost identical, as are their distributions along the path running down the length of the conducting bar. Now, what is the physical significance of TENE? The MKS units of TENE appear to be W-K (watts times degrees Kelvin or Centigrade). This does not seem to have direct relevance to Joule heat or even to thermal conduction, though it may be more-closely related to the latter. Additionally, it does not have units of energy, so its name is perhaps misleading. It may be a convenient way to assess/quantify discretization error, but has little practical engineering value.
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?