January 25, 2023 at 7:16 amFAQParticipant
Problems arise in TurboGrid when using the ATM method with a turbine that involves 2 unique blades in the blade set. When there are 2 unique blades, it results in 4 possible blade configurations: 2 for the blade order and another 2 for the mirrored configurations. In most cases,there are 2 templates—one for each blade order. To handle the mirrored configurations, the theta direction in TurboGrid must be reversed. In the cases where there is only 1 template for blade order, the template may be meant for one direction while TurboGrid is trying to use it for the other. This causes the topology to not be placed properly on the leading edge of the main blade. Note: The longest blade should always be the first blade in theta order. To use the ATM method with this type of case, the following approach can be implemented: 1.Edit the original BladeGen file: Reverse the flow direction Reverse the rotation direction Flip the angle sign convention by going to Model > Coordinate System Orientation > Left-Handed 2.Export the geometry to a Neutral Data File (NDF): Go under Blade Properties > LE/TE Ellipse tab and switch the Ellipse location from “tangent” (i.e. bottom radio button) to the top selection to allow the NDF to be exported Export an NDF 3.Create a new BladeGen cell in Workbench: Drag out BladeGen into Workbench Open the NDF created earlier under File > Open Go under Blade Properties > LE/TE Ellipse tab again Toggle the radio button for Ellipse Location back to the bottom location (the original tangent option) 4.Connect TurboGrid to the new BladeGen cell in Workbench and generate the mesh
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.
- ANSYS Fluent: Introduction to the GEKO Turbulence Model Part I
- Delete or Deactivate Zone in Fluent
- What is meant by Warning: Flow boundary zone 18 is adjacent to a solid zone?
- ANSYS Polyflow: Adaptive Meshing Based on Contact
- Aero-Mechanical Simulation of Turbomachinery Blading
- Apply Custom Material Properties in Fluent
- ANSYS System Coupling: Two Way Fluid Structure Interaction – Part 1
- Predict Gearbox Lubrication, Oil Temperature and Churning Losses using CFD Simulation
- Check CPU Time in ANSYS FLUENT
- How to Predict Performance of Bioreactors and Mixing Tanks