June 14, 2023 at 1:03 ammasud407Subscriber
Can anyone of you tell me how I can apply spatially varying loads (for 3D) on each node using ANSYS workbench? For example: the load varies for each of (x,y,z) coordinate.
June 14, 2023 at 10:57 amSaurabh PatilAnsys Employee
You can find more detailed guidelines on applying spatially varing loads on this Ansys Help Document pages.
Let me know if this helps you out.
June 15, 2023 at 11:06 pmmasud407Subscriber
Unfortunately, I can't access into the link as I do not have the customer service account
June 16, 2023 at 7:41 amj_pAnsys Employee
To apply a spatial varying load or displacement in Ansys Mechanical, you must first generate the mesh, and then specify the Magnitude property of the variable load, or the load input, as Tabular (see below) or as a Function and then specify the desired coordinate (X, Y, or Z) for the Independent Variable property.
To select the desired nodes simply choose the associated selection tool, as shown here:
If you would like to apply spatially varying loads to multiple nodes in your mesh, it might be worth considering to write your own subroutin/commands, using e.g. PyMechanical documentation 0.9.0 — PyMechanical (pyansys.com).
I hope this helps.
June 16, 2023 at 4:29 pmmasud407Subscriber
If I select the tabular data, it provide me the option for time vs pressure data. But I want to insert load for each node (X,Y,Z). So the data table needs to be have (X,Y,Z) and P, which I cant define.
June 19, 2023 at 6:44 amj_pAnsys Employee
If you select a (nodal) force from the list of boundary conditions, you will also be able to supply tabular data for P in x,y and z.
You can also apply direct FE type boundary conditions to create spatically varying nodal forces (for Static and Transient analyses only), by clikcing on the Environment Context tab, then click on Direct FE > Nodal Force. As a scoping method you will have to use a Named Selection, as shown below
Subsequently, you will be able to enter a magnitude for the x, y and z component to define the load, e.g. like
June 19, 2023 at 9:36 pmmasud407Subscriber
Does this X, Y,Z denote the cooredinate? I think it denotes the X, Y,Z components of the force. I need to apply forces at various coordinates (X,Y, and Z).
June 20, 2023 at 7:52 amNickFLSubscriber
One way to do this would be to use External Data on the project page. You would then import a simple text file, csv or something similar, with x, y, z points and then the forces Fx, Fy, Fz. When you load in the data in External Data, you can define the columns as Coordinates and then the others as Forces. The force ones will be give a name like File 1:Force 1, File 1: Force 2, etc. Then you can go into Mechanical (make sure you create a link between the external data and the static structural on the WB page) and then apply this Imported Load on the required face. You can set the interpolation method and even visualize the imported load. You won’t likely want to do a direct nodal force as if you change your mesh then you would have to regenerate the forces all over. A sufficiently fine Interpolation file is more valuable.
I would recommend you do a test case on a simple inclined plate before moving onto your actual geometry. It is easier to understand and debug when you have simple geometry.
July 6, 2023 at 8:42 pmmasud407Subscriber
Mr. NickFL, thanks for your suggestions. I was trying your approach and have some follow up issues. First of all, I can assign different X,Y,Z values, but there is column for force or pressure (but no option to specify Fx, Fy, and Fz separetely). Then when I apply that external force (imported load), I can only select a face (not the whole volume). Now my question is the force applied normal to that selected force?
Then I tried to apply stress in place of force, in this case, I can select the whole volume. But what does this stress means? Is it an input as von-mises stress or any of the principal stresses?
July 10, 2023 at 7:32 pmNickFLSubscriber
Sorry for the late reply. I have a broken elbow, so I am typing like a rooster.
And sorry, again, for recommending pressure (surface force) when you clearly had a volumetric force in the title. Instead of having forces, you will have a force per volume (such as N/mm³). This is typically used in Emag simulations. When you create the csv with the appropriate units, there will be the option to use the applied imported load as a body force density (or volume force density-I cannot recall the terminology Mechanical uses). There can be a force density in each component direction. This was added in a recent version of ANSYS, so if you are using an old unsupported version I recommend you upgrade.
To understand why you need a force density and not just the forces, consider the following thought experiment. If you have a linear cube element, and you applied 1 [N] at each node, you would have 8 [N] acting on that element. If we use a finer mesh, so two elements in each direction, we then end up having 27 nodes and therefore 27 [N] applied. We are solving a different problem! By using the force density, the smaller element size will shrink the applied force on each node. ANSYS is great in that it keeps all the bookkeeping hidden from us. That is why we pay the big bucks for the software--not to have to consider such things.
What physical process are you modeling to have these external forces?
June 19, 2023 at 9:37 pmmasud407Subscriber
Also, I need to apply loads at all the grid/node points. Each node will have different magnitude of forces.
- You must be logged in to reply to this topic.
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.
- How to work with STL file?
- Rotate tool in ANSYS Design Modeler
- section plane
- Using Symmetry in DesignModeler and Expanding the Results
- ANSYS FLUENT – Operation would result in non manifold bodies
- drawing a geometry by importing a table of points
- material properties
- Coordinates orientation
- “contact pair has no element in it.” how to resolve this problem
- Parameters not imported into Workbench 18.2 from Solidworks/Inventor
© 2023 Copyright ANSYS, Inc. All rights reserved.