Forces/Pressures in Hypermesh

Altair Forum User

Hey Guys,

I am an undergraduate student of Mechanical Engineering at the University of Michigan and am doing HyperMesh analysis for the Solar Car team.

I have done some basic analysis on different parts of the car by meshing them then using constraints/forces then using NASTRAN for the actual FEA.

At the moment, I am trying to set up the analysis for the rims of the car for analysis however I need to apply a uniform pressure/force caused by the tires on the actual rim. However, I am not sure how to do this because the pressure/force can only be in one direction, but I want the load to point to the center of the rim as that is the correct direction. Is there a way I can do this? Or do I have to resort to selecting each node individually and applying forces to it?

I have already:

1. Meshed the rims

2. Set up all the collectors

Now all is left is to input forces/pressures so that I can run the analysis.

On a side note are there any good tutorials on how to analyze assembly's in HyperMesh?

Any help would be much appreciated.

Thanks,

Apoorva Bansal

B.S.E. Mechanical Engineering & Computer Science

University of Michigan

Altair Forum User

Hi Apoorva,

For this, you need to create a cylindrical coordinate system local to the Rim and then apply the forces on this local system.

Could you please follow the procedure that follows?

1) Go to Analysis Page > Systems panel > create by node reference sub-panel >Switch entity selector to cylindrical. Specify the origin node, z-axis node & xz-plane node. Specify the appropriate system size and click on create.

2) Now switch to assign sub-panel in systems panel. For the set: option, select the nodes on the circumference of the Rim and assign them to the cylindrical system created for the to: option.

3) Remaining in the analysis page, go to forces panel > create sub-panel and select the appropriate nodes. Toggle the system to local system and select the cylindrical system created. Specify the appropriate magnitude, direction etc. and say create.

Altair Forum User

I'm working on a similar problem as Apoorva. Is there a way to apply a nonuniform circumferential loading around the rim. I would like something like a sinusoidal load distribution around the rim.

Thanks,

Mike McLeod

Altair Forum User

For Apoorva's original question:

Keep in mind that what HyperMesh will visualize doesn't always match what the solver code expects. For pressures, the HM panel 'pressures' requires a list of elements to apply the pressure to, a direction, magnitude, and a list of nodes on the face or edge. The vector created will be oriented in the direction you chose. However, NASTRAN actually applies the pressure load normal to the element face, using 4 grid points (HyperMesh will list the 4 grid points at the corners of each element). The direction that you choose to define the pressure load isn't used, other than to draw the vector visually.

For Mike:

To get a loading that is easily defined as a math function, but not so easy to define manually over a series of nodes, try the 'field loads' utility. This is included in the hm/scripts/dlm directory of the HM9 installation, and you can activate it by adding the following to your userpage.mac

*createbutton(5, 'Field Loads...      ', 0, 0, 10, BUTTON, 'Create load by equations.', 'tcl_script', 'mathbc.tcl')

Cheers,

Eric