Plate Forces and Moments – Intro:
You may have heard these terms related to plate forces and moments:
- Membrane loads
- Transverse shear loads
- Bending moments
These terms refer to the plate forces and moments (plate/shell elements or laminate elements). But primarily, we will be focusing on FEM application. Althoough they are expressed as resolved running forces and moments, they come from what are called “Stress Resultants” and they are expressed in equivalent load and moment units per unit element edge length.
Plate elements are the most commonly used finite elements to model sheet metal or plate type structures. In case of laminates or sandwich panels, their finite element formulation is also based on the same basic plate theory. Except in laminates, different plies or layers with different material properties, orientations and other characteristics are accounted for. Here is a good link that goes into a lot of detail on the mechanics of laminates: Basic Mechanics of Laminates
The same link is also available on our Engineering Resources page along with many other useful links, so check those out too. But in this post, we will focus on the FEM analysis output file and the plate forces and moments written to the output file. So it behooves us to understand the plate forces and moments and how to interpret them.
Plate Forces and Moments Schematics:
- NX is positive going along the element X axis
- NY is positive along the element Y axis
- NXY is positive along the counter-clockwise right hand screw rule direction about the positive element Z axis
- QX/QY are positive along the element Z axis
- MX, MY and MXY are positive as shown below, for example MX is positive if it produces tension (along +NX) on the positive side of the element
- Also note that NXY = NYX and MXY = MYX
The following figure illustrates the membrane loads and transverse shear loads on a plate/shell/laminate element. By ‘membrane’ loads, we mean these loads are acting in the plane of the element. By ‘transverse’ loads, we mean these loads are acting out of the plane of the element. Axial loads NX and NY are shown according to the right hand screw rule convention. NXY is the in plane shear load. QX and QY are transverse shear loads. All the loads have the units of lb/in (element edge length) in English units.
These loads include applied loads (nodal, inertial, pressure etc.), and loads from the adjoining elements. The schematic shown above is a free body diagram of this element. All the forces balance each other for static equilibrium.
It is also important to note that all these loads are written out to the analysis output file at the mid-plane or Surface-0 of the elements as ‘running’ (load per unit edge length) loads.
There are also grid point forces that can be written out using the “GPFORCE” case control card’s print option in nastran. These loads are nodal loads that satisfy the grid point force balance from all elements connected to that node.
Similarly, we also have the plate element bending and twisting moments. These moments are shown in the schematic below.
Note: In general, when we talk about basic engineering mechanics, MX is a ‘moment about X’. But here, MX means a moment that is acting in a plane that is perpendicular to element X axis and MY is a moment that is acting in a plane that is perpendicular to element Y axis.
In the figure above, we can see the various bending (MX and MY) and twisting (MXY) moments. The same balancing and units (lb-in/in) principles apply to these moments as well. MX and MY try to bend the plate, while MXY tries to twist the plate.
Finite Element Analysis – Element Forces:
So how can we make sense of these loads and moments in a practical sense? The best way to do that is to experiment with a sample test model. To keep it simple, we will focus on the element forces.
Let us build a simple 0.063″ thick 4.0″x4.0″ square plate made from 2024-T3 aluminum alloy. An element size of 0.5″ is used creating all square elements. The model is shown below with thickness turned on.
The three nodes at the left side are fixed, the three nodes at the right are loaded as shown. This is a thin plate so it does not take much load to bend it.
The sequence of steps is as follows:
- Run this model (SOL 101)
- Make sure GPFORCE and FORCE “(PRINT)” options are turned on in the case control of the input deck
- Select an element somewhere in the middle
- Display its freebody nodal loads
- Sum the nodal loads along element axes at the two nodes on either side of the element
- Then divide the total load on either side of the element with the edge length between the two nodes
- Thus, we get the ‘running’ loads NX NY NXY QX and QY
- We then compare these numbers to what is written out to the output file at the center of the selected element
PHEW! That was a of steps. But don’t worry, the figure below shows the freebody display of element ID 29 after the above steps are done.
Element 29 Freebody Loads:
The figure below displays the freebody loads on element ID 29. This element was chosen due its location being close to the center of the plate. The idea is to look at a far field element from load and constraint locations.
Considering element ID 29, we can see that the X load at nodes 50 and 59 balance those at nodes 45 and 46.
Any Element Edge Length = 0.5"
At nodes 50/59:
Total X Load = 58.555 lb + 58.57 lb = 117.125 lb
NX = 117.125/0.5 = 234.252 lb/in
At nodes 46/45:
Total X Load = -59.267 lb - 57.859 lb = -117.125 lb
NX = -117.125/0.5 = -234.252 lb/in
So NX is balanced on either side. Same calculations apply to all the other forces.
Element 29 Output File Force and Moment Values:
Now we need to check and see if these force values are reported at the center of this element in the output file.
The figure below shows the plate forces and moments for element ID 29.
We can see in the figure above that the FX or NX value matches with the calculations from the element 29 freebody display we saw earlier. The moments may have similar calculations, but I might do that part in a later post, haven't figured that one out yet.
How do you use these plate forces and moments in actual stress analysis hand calculations? Well, this will be covered in future stress analysis courses.
So there you have it. If you have any comments on this make sure you let me know, comment below...
If you like this post, then subscribe below to get instant updates on future posts like this: