Load Panel in Mecway

Vinicius_Petrucci

this would be possible on the mecway, is there any strategy?

Load to panel nodes
Panel of this type transfers the applied load to all or selected nodes (corners) of the panel. The load is generated only in supported nodes. Sum of load is transferred to nodes according to the length of edges connected to each node. The user can set the weight for individual nodes or exclude some of them from load transfer.


Load to panel edges
Panel of this type transfers the applied load to all or selected edges of the panel. The load is generated only along supported edges ("supported" means supported by another member, it is not possible to define a direct support on the load panel). Sum of load is transferred to edges according to the length of edges. The user can adjust the weight for individual edges or exclude some of them from load transfer.

Victor

Load to panel nodes:

• If the geometry is simple (axis aligned, not too many nodes), it may be practical to do it using constraint equations.
  
• With the CCX solver, there's the *DISTRIBUTING COUPLING keyword which also requires you to specify the weights, including the length relationship.
  
• With CCX, there's also node-surface coupling which includes the lengths automatically but you can't specify custom weights or exclude nodes.
  
• If your aim is to apply a load to an arbitrary location on a surface independently of the mesh, another way is using a pressure load (which optionally doesn't have to be normal to the surface) with the unittriangle() function, or two of them for a 2D surface which distributes the load over an area and puts the line of action at an arbitrary location you choose.
  

Load to panel edges:

• The first two options above might be useful.
  
• There's also line pressure which distributes a load uniformly along an edge but it doesn't exclude "unsupported" edges nor allow custom weights.
  

Victor

An additional thought -

If the load should be distributed according to the area of the panel such as uniform pressure load a floor, then my previous suggestions are probably too complicated and the only practical option may be to mesh the panel explicitly. With the internal solver, you can connect a shell element panel to a beam element frame using bonded contact so you don't have to worry about making the meshes compatible. You might have to tune the panel's stiffness to make it behave more like an ideal zero-stiffness load distributer. With linear analysis, this could be done simply by giving it a very low thickness and/or Young's modulus.

For "Load to panel nodes", you could connect the panel elements to the supported nodes using beam elements to give you control over how it's distributed to each node (the weights).

Vinicius_Petrucci

Victor, this additional answer helped me.
thanks