Learning Forum

[masud407]

Hello, 

 

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.

[Saurabh Patil]

Hi masud407

You can find more detailed guidelines on applying spatially varing loads on this Ansys Help Document pages. 

https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v231/en/wb_sim/ds_spatial_load.html

https://ansyshelp.ansys.com/Views/Secured/corp/v231/en/wb_sim/ds_spec_load_values.html#ds_Spat_load_dis_fctn

Let me know if this helps you out. 

 

Regards

Saurabh

 

[masud407]

Unfortunately, I can't access into the link as I do not have the customer service account

[Janos Plocher]

 

Hello masud407,

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.

Regards,

János

 

[masud407]

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.

[Janos Plocher]

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

[masud407]

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).

[NickFL]

 

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.

 

[masud407]

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?

[NickFL]

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?

[masud407]

Also, I need to apply loads at all the grid/node points. Each node will have different magnitude of forces.