September 27, 2017 at 11:19 amadminAnsys Employee
What are the definitions of Body coordinate and Global coordinates systems used in ANSYS FLUENT 6DOF model?
November 8, 2017 at 8:12 amVishal GanoreAnsys Employee
The global coordinate is same as computational domain coordinate system. The body (local) coordinate is fixed to the body. The body coordinate is defined by providing the C.G values and C.G orientation (not necessary that c.g is inside the body). This is with respect to global coordinate system. During the calculation, the body coordinate changes (as the body moves), so the c.g and c.g orientation (global coordinate). Once the body is moved, all these values (c.g, c.g vel and c.g orientation) on the global coordinate will be updated in the panel. All the values in the 6DOF panel (cg, cg velocity, and cg orientation) are with respect to global coordinate system. The C.G orientations are Euler angles. The order uses the right hand rule based on the positive rotation axis. Rotation about X (Y to Z), rotation about Y (Z to X), and about Z (X to Y). The c.g. orientation is used to compute the transformation matrices. Fluent calculates angular velocity and acceleration on the body coordinate system and internally transforms to global coordinates to return to fluent (uses transformation matrices). The external moment and forces can be given on the local (body) or global coordinate system using the macro prop[SDOFLOADLOCAL]. The boolean "prop[SDOFLOADLOCAL]" can be used to determine whether the external forces and moments are expressed in terms of global or body coordinates. TRUE for local /body coordinates and FALSE for global coordinates. Default values is FALSE. Moment of inertia provided in the UDF should be at the c.g of the body ( i.e. on the local (body) coordinate system). The C.G and C.G orientation in the 6DOF panel fixes the body coordinate system. If both are zero initially, that means both coordinate are same at time=0.
January 30, 2019 at 3:03 pmusamaSubscriber
I need your help regarding VOF, open channel, moving mesh problem for the filling of microcavities. if you help me with this. it will be appreciated.
December 4, 2019 at 10:00 amshubhamkhodiyarSubscriber
I am working on the problem, where two bodies are connected by a hinge joint, moving underwater. The motion of both bodies is governed by SDOF properties. To model the hinge joint I am using "relative motion" option in dynamic mesh zone dialog box, I want to know whether relative motion option take care of forces being transferred between the bodies due to joint. If not how can i dynamically couple the bodies
How can we access the acceleration of the body at any time step in UDF to calculate inertia force?
- The topic ‘Definitions of Body coordinate and Global coordinates systems used in ANSYS FLUENT 6DOF model’ is closed to new replies.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- legend min and max
- Ensight hot iron palette from an image
- Streamlines in EnSight using MRI data
- Import MRI data into Ensight
- FLUENT APPLICATIION ERROR
- Total Surface Heat Flux Calculation in Fluent
- Drop Test of a Water-Filled Tube
- Difference between “total pressure” and “absolute pressure”?
- obtaining pressure distribution by making points in ansys
- Minimum Orthogonal Quality Less than 0.01 For Transonic Airfoil Flow Analysis
© 2023 Copyright ANSYS, Inc. All rights reserved.