Learning Forum

[chasha19]

Hello,

I am new to AnSys, I am using AnSys 2020 R1. I am trying to apply loading to a part for the purpose of deformation and stress analysis. This particular part is an aluminium rocker which is supported by a central bearing, and has two push rods loading it via spherical joints.



What I'd like to analyse is a scenario when the push rods each apply 800N parallel to the plate surface, perpendicular to each other.

My current method of analysis (unsure if best), is to 1. set the support to cylindrical support (largest hole in the part), and then 2. insert bearing loads at each joint. The confusion I have is related to this bearing load and how to set the vector.

What I've done is select the two faces of the cylindrical surface, and inserted the bearing load with those selected. I then enter my magnitude at 800N. I notice at this point that the direction of the load is always generated as being parallel to the surfaces i have selected. This seems very strange and counter-intuitive to me. The way that I rectify this is to deselect defined by "vector" and select "components", at which time I enter my X Y components and leave Z at 0. This is shown in the next two screenshots.

What I'd like to know is if there is a less counter-intuitive way to set the force vectors. Perhaps I can introduce an arbitrary axis (or two) into the model (perhaps in the geometry phase of the simulation?) which I can then apply my vector to at this later stage? Or, is there some setting i can change that stops the force applying parallel to the surface I select for it?

Thank you

[peteroznewman]

Using Components is the right way to go if no geometry points in the direction you want to specify.  You can create a new Coordinate System that is rotated to the right angle so the components are only X or only Y.

You shouldn't apply two forces to a rocker that is supported on a center bearing, because the structure is still a mechanism with one degree of freedom: rotation about the axis. The result of that is a pivot error in the solver unless Weak Springs are used. Instead, one arm of the rocker should have a remote displacement that has a single displacement degree of freedom set to 0 while all others are Free and that direction is tangential to the rotation.  The other arm has the force applied.  You Probe the Reaction Force at the arm with the Remote Displacement to see that the force is the expected value.

I recommend you use mesh Method of Sweep and put 4 elements through the thickness, or use a midsurface to replace the solid.

[chasha19]

hello peteroznewman,

thank you for your reply. Can you explain how to create a new coordinate system that is aligned at any desired angle? This would save me doing trig.

Another related question: I have construction lines (a sketch) in my solidworks model which could define the vectors applied to the rocker. Is there a way to import these construction lines into the geometry that is analysed by AnSys (with the hope of applying a bearing load vector to that construction line)?

[SaiD]

Hi,

With respect to creating a coordinate system aligned with a desired direction, please go through: https://www.youtube.com/watch?v=SdvipBnni1E

Some of the options may be located in a different location (since the video shows an older version), but you should be able to use the Transformations to rotate the local coordinate system by any angle you wish.

Hope this helps,

Sai

[chasha19]

Thank you very much Sai