Why am I getting different results for plane13 and plane223 ————————————————————– I created a simple structural-thermal static coupled analysis. In the first example a plane 13 is used, in the second one a plane 223. These are identical 2D axisymmetric models of a disk spinning at 200 revolutions per second and at 1000 C above the reference temperature. Material properties are orthotropic but linear. Using orthotropic properties, the results differ substantially (the PLANE223 model is correct). If materials are isotropic, there is no difference in results (both models are correct). Further testing: testOrtho_2D_af_13.txt: PLANE13 model testOrtho_2D_af_223a.txt: PLANE223 model, matrix coupled thermal and structural matrices testOrtho_2D_af_223b.txt: PLANE223 model, load vector coupled thermal and structural matrices testOrtho_2D_af_223c.txt: PLANE223 model, load vector coupled thermal and structural matrices with NSUB,2 to force more than one iteration for (hopefully) proper coupling. As you can see from the attached plots, only the direct coupled method (â€œ223aâ€ files) appears to give sensible results (we expect tensile radial stresses about a third of the way from the center of the disk, NOT negative ones as determined by all the load vector coupled models).
March 17, 2023 at 8:59 amFAQParticipant
The issue seems to be related to a misinterpretation of the TUNIF functionality. According to the TUNIF command description, its behavior varies depending on whether the analysis is simultaneous or iterative: “Since TUNIF (or BFUNIF,TEMP) is step-applied in the first iteration, you should use BF, ALL, TEMP, Value to ramp on a uniform temperature load.” In other words, when the analysis is simultaneous (matrix coupling between U and TEMP using keyopt(2)=0 with PLANE223), the temperature nodal load is zero (TUNIF ramped) andthe thermal strain EPTH is zero (since TREF=0). These are the results the user wants to see. However, when an iterative analysis is activated (load vector coupling using keyopt(2)=1 with PLANE223 or PLANE13), the temperature nodal load is 1000 (TUNIF stepped) and thermal strain EPTH = ALPH*1000 is non-zero . To achieve the desired results with a load vector coupling, the user must either use the bf,all,temp,1000 command instead of tunif,1000 or issue tunif,1000 together with tref,1000. I have attached an additional input file (testOrtho_2D_af_223d.txt) which uses load vector coupling, replacing TUNIF with BF,ALL,TEMP,100. The results are now the same as they were for input file testOrtho_2D_af_223a.txt (which is to say they are now correct).
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.