Plate or shell elements are useful for modeling the stiffness characteristics of walls, slabs, roof systems or other flexible diaphragms either in bending or in shear. Mathematically plate elements are thin, 2D areas that may be represented as quadrilateral or triangular shapes--they do not exhibit through-thickness stress variations like a 3D "brick element" would. Nonetheless, they are extremely useful for modeling many civil/structural problems.
While plate elements may be created manually, using an Area object with meshed plates is generally more convenient. Auto-meshed areas require the advanced level of VisualAnalysis, but offers more flexiblilty with modeling, separation of loads from plates, makes it easier to reconfigure your model or perform mesh refinement.
Unlike member elements for static analysis, plate elements (manual or auto-meshed) are always approximate: you must use mesh-refinement techniques to know if you have enough plates in your model. Plate elements are rarely used as single elements, but are more often used as a mesh; generally the more plate elements you use, the better accuracy you get.
- Create plates by sketching, the tab in , or through importing DXF, etc.
- Uses for Plate Elements: walls, slabs, roof systems
- Element Formulation: bending and membrane behavior, thick elements
- Thickness: out-of-plane thickness
- Shapes: triangular or quadrilateral
- Materials: See Member Materials
- Connections: rigidly connected to nodes, ONLY connected at nodes!
- Local Coordinate System: local x,y, and z directions
- Behavior Related to Structure Type
- Meshing: Mesh Refinement, convergence, how many plates are enough?
- Load Types: out-of-plane pressures
- Results: in-plane stresses, bending forces and shears, units, sign convention
- Auto-Meshed Plates vs. Manual Plates
- Complex Systems: stud walls, stiffened plates, corrugated metal deck
Uses for Plate Elements
You can use a mesh of plate elements to model a concrete floor slab or you could use multiple meshes in various orientations to model the flanges and webs of a wide-flange steel beam, perhaps to investigate localized stresses near some coping or holes. The use of plate elements is sometimes as much art as it is science and you are encouraged to get a good book on FEA modeling to understand some of the nuances.
Distributing loads is possible through a complex plate mesh--but NOT through a single plate element. A better choice for load distribution is an Area.
You could use plate elements to model the stiffness of something that you are not really investigating directly. For example, you could model a flexible roof diaphragm with a minimal number of membrane-only plate elements between the framing members of the roof to simply help the model hold its shape and transfer in-plane forces. In doing so you are not accurately modeling what is happening inside the diaphragm (which might be some very complex system of orthotropic materials or construction!), but you are modeling the overall behavior.
There is always a trade-off of performance vs. accuracy when using plates. The more you use, the better (generally). But the more you use, the slower the analysis, the longer your reports, and the more time it can take to manipulate and check your models.
Plate Element Formulation
A plate element will account for bending with transverse shear effects in thick plates and rotational drilling degrees of freedom. It is important to note that these formulations are not coupled during the initial analysis. The stiffness matrix for each formulation is computed separately in local coordinate space. The two formulations are assembled into a total 6 degree of freedom (dof) global element matrix. Once assembled into the global element matrix, the element is combined into the total structural stiffness matrix. Membrane and bending coupling is achieved with the addition of geometric stiffness terms in the overall stiffness matrix. The additional stiffness terms result from membrane strains which are calculated during the initial analysis. Once the membrane strains are found the element stiffness is automatically updated to account for the extra stiffness terms resulting from membrane strains.
You can turn off bending behavior to create membrane-only plates, find the option in thetab.
Both the membrane and bending formulations are based on triangular elements. When you use a quadrilateral element, internally four triangles are used with a middle node which is removed through static condensation thus creating the quadrilateral. Unlike in the past, with a constant strain formulation, triangular elements are very accurate in VisualAnalysis.
Bending: Thick-Thin Triangle (Xu)
The bending part of the plate element is now based on the triangle formulation originally presented by Xu et. al. in 1992, which includes transverse shear effects. Prior versions of VisualAnalysis and many finite element analysis packages use the discrete Kirchoff triangle (DKT) as their primary thin plate element. Although the DKT element is a reliable and widely used element for plate analysis, it cannot accurately model thick plates. The new element accounts for transverse shear effects present in structures that might contain areas with thick plates, such as footings or thick floor slabs.
Xu, Zhongnian, "A thick-thin triangular plate element" International Journal for Numerical Methods in Engineering, v. 33, 963--973 (1992).
Membrane Formulation: Allman Triangle
Drilling degrees of freedom, previously unavailable in VisualAnalysis, have been added to the plate element resulting in a 3-dof per node plate element. This means that you may apply a moment perpendicular to the surface of the plate element at any of the three (triangle element) or four nodes (quad element). Elementary membrane elements ignore drilling dofs in order to avoid membrane locking. However, drilling dofs are part of many structural engineering problems.
Membrane locking in the new element was avoided by independently interpolating the drilling rotations over the element and introducing a penalty stiffness based on the shear modulus. The membrane element presented in VisualAnalysis is based on the early work of Allman. The element is similar to the standard CST membrane element but includes an additional rotational degree of freedom at each node. We use 4-point symmetric integration using the points from Cook, which gives good results and matches the data from Allman's paper. Drilling DOF in membrane elements are difficult as all elements exhibit "membrane locking" and zero-energy modes, these issues can become very prominant in coarse meshes.
D. J. Allman. "A compatible triangular element including vertex rotations for plane elasticity analysis.", Computers & Structures, 19(1-2):1.8, (1984).
Robert D. Cook, Concepts and Applications of Finite Element Analysis, 4th Edition, Table 7.4-1, (2001) ISBN 978-0471356059
You can safely model both thin and thick plates in VisualAnalysis. Thick plates automatically include the effects of transverse shear deformations important for modeling foundations and footings.
Plate elements can be quadrilateral (4-nodes) or triangular (3-nodes) in shape. The element formulation is good enough that you do not generally need to worry about making the quadrilateral elements square. Elements may be distorted significantly without problems. We have run tests comparing the results of long thin elements and they work well—to a point. For the very best results you should keep the element aspect ratios close to 1:1, but you should not expect any problems with ratios of 5:1 or even higher.
Unlike member elements, plate elements are always assumed rigidly connected to the nodes in all directions. There is no provision for partially restrained (PR) or plate element releases at their connections.
For efficiency reasons, you should avoid situations where you have dozens, or hundreds of plate elements all connected to a single node. This situation commonly happens at the center of a circular disk, with radially generated plate elements. You may wish to adjust the mesh near the center to alleviate the situation.
Plate Local Coordinate System
Plate elements have their own local coordinate systems. The local system has its origin at the centroid of the plate. The local x-axis is parallel to and in the direction of a vector from the first node to the second. The y-axis is perpendicular to the x-axis and in the plane of the plate. Note the right-hand rule where the local z-axis points out of the plane defined by the counter-clockwise node ordering. The picture below clarifies this, using a triangular plate element as an example.
For plate elements, the local systems are used for directing pressure loads. Local forces and stresses are also reported in these directions. From a practical standpoint, it is usually necessary to be consistent in the creation of plates. The convention is to draw elements in a counter-clockwise manner, from the lower left. Generated plate elements in VisualAnalysis are usually oriented this way. You can use the Filter tab in Project Manager to show plate local coordinates to verify their directions.
As mentioned, the local coordinate system becomes very important when applying plate pressures. If the plates are randomly drawn in either direction the local z-axis will point in opposite directions and loading will become rather difficult.
Plate Behavior and Structure Type
Plate elements exhibit two general behaviors depending on the structure type. The first behavior develops membrane stresses which are in-plane stresses resulting from stretching, compressing, or shearing the element. The second behavior develops bending stresses which are the result of out of plane pressure loads or rotations out of the plane. The structure type will dictate which of these behaviors are present.
& Structure Type
Meshing, Mesh Refinement
One of the more difficult tasks you have as an engineer is to verify the validity of your results. Plate elements are approximate—the more elements you use, the better your results. There is a tutorial project called Element Mesh Demonstration, installed in the Examples folder, to demonstrate this concept.
Meshing is simply using multiple (many) plate elements to model a wall or slab rather than just one. You can draw one and then manually split it. If you have the advanced level Auto-Meshed Areas offer many advantages. When manually creating a plate mesh, take care to align the elements such that the local z axes are all pointing in one direction!
Determining a plate element size that gives accurate results and minimizes your model (and your time) is critical. VisualAnalysis uses a plate element with good convergence characteristics. Use the following procedure to minimize the number of plates in your models:
Plate Modeling Procedure
- Start with an element size that matches the natural geometry in the model. Use nodes at locations where other plates connect or where members connect. Try to minimize the number of plate elements in a reasonable way—do not bother with a single plate, though!
- Run the analysis and record your results. If you have reason to question the results or if you have no way of knowing whether or not they are reasonable, proceed to step 3.
- Subdivide your initial element meshes into smaller elements. Model | Split Plates makes this process easy. Analyze again with the refined model.
- Compare the results of step 3 with the previous analysis. If the results
are similar, assume you are near the converged solution and feel somewhat
confident of your results. Otherwise, if the results differ substantially,
return to step 3.
How Many Plate Elements are "Enough"?
The following picture shows what happens as you "refine" your model by using smaller elements. Your goal is to get into the "flat area" for the model, the area where results do not change much as you refine the model further.
As a general rule you will want to place more elements in areas where stresses and forces in the plates are changing the most per unit length of mesh. Stress concentrations or locations near concentrated loads may require smaller element size. At locations under uniform loading/no loading, and away from geometric irregularities, large elements may be sufficient.
Plate Load Types
While you can apply loads directly to plate elements, it may be easier and smarter to apply your loads through an area that "covers" the plate elements. This allows you to separate the loading from the finite element model and allows you to re-mesh the plate elements without redefining loads. Modeling changes become more independent of loading.
Plates may be loaded with a perpendicular pressure or a thermal change. Pressures and thermal gradient loads will cause bending in the plate, and are only available for 3D models and the Plane Grid.
Plate pressure loads are applied using a technique of equivalent nodal loads--meaning there is no actual load applied to the plate element itself! This means that loading a single plate element will not have any direct effect on that plate. Because of this, using a single plate element (vs. a mesh) for distributing loads is not useful or wise.
Plate pressure loads act only in the local z-axis, or perpendicular to the plate. These loads may be uniform, linear or warped. There are two ways to define plate pressures. First, you can define the load on an element-by-element basis, where pressures are specified for each corner of the plate.
Mesh Linear or Hydrostatic Loads
You may apply a linear or hydrostatic load to an entire mesh of plates, where the load is defined based on global positions and directions and the individual pressures on each element are calculated automatically. Internally the load is applied individually to each plate element, but the definition of the load is easier to understand. Once applied you may edit or delete individual loads on plate elements, or edit them as a group by selecting them all together.
Plate elements may also resist thermal loads. Currently both a temperature change load and a temperature gradient load may be applied. The temperature change load acts uniformly through the thickness in all directions. The net effect of this type of load is a stretching or shrinking in the plane of the plate. A gradient load is a linear varying temperature through the thickness. This load is specified as a change in temperature, dT. The top surface is set to dT/2 and the bottom surface to –dT/2. This load causes pure bending.
Edge or Side Loads?
There is no way to apply edge or side loads directly to plate elements in VisualAnalysis. You can apply nodal loads to all the nodes along the edge of a plate mesh, or you could create a "dummy" member element along an edge and then apply loads to that--pay attention to weight and stiffness of this member!
Perhaps an easier alternative is to use a Meshed Area and apply a Side Load to the area, this requires the advanced level of VisualAnalysis.
Plates can report moment and shear forces for out of plane bending, and normal or shear stresses for in-plane activity.
Plate forces and moments are reported per unit length of plate, moments have units of force*length/length and shears have units of force/length. Plate membrane stresses may also be output relative to the global or local axes.
Local Plate Results
The sign convention for moments: a positive moment produces tensile stresses on the +z local coordinate face of the element, as shown in the sketch. This is typical plate notation as found in most texts on plate theory.
The picture below shows the sign convention for positive stress directions. As usual, positive normal stress indicates tension.
If plates in your structure can also bend, stresses may be reported at each of the top and bottom faces. Stresses at the face are combined bending and membrane stresses. If plates are subject to bending stresses only, the mid-plane is the neutral axis and therefore the normal stresses at this plane will be zero.
Global Plate Results
Plate forces and stresses may be reported with respect to the global coordinate system. This simplifies result interpretation when the local axes of elements in a complex mesh are not identically aligned. The global forces follow the right-hand-rule for sign convention. That is, a positive MX moment is at the global X edge of the plates and rotates about the global Z-axis. Some results may be zero after the transformation to the global directions, for example the global-Z moment for a mesh lying in the X-Y plane.
Plate results may be seen graphically in Result Views, or tabularly in various report tables.
Yield Stress: Von Mises
The report for Plate Principal stresses includes the calculation of the Von Mises "effective stress" or yield stress:
"Von Mises" = sqrt( 0.5*((s1 - s2)^2 + s1^2 + s2^2) )
where s1 = principal maximum stress, s2 = principal minimum stress. Note that s3 in VisualAnalysis is zero because we are using a thin-plate element with no through-thickness stress, so the equation is simplified from the general one.
Meshed Plates vs. Manual Plates
VisualAnalysis can automatically create plate meshes, through Areas, and this can greatly simplify the work you have to do in modeling. Automatic or meshed plates are managed by the system and will provide good connectivity with any members, manual plates, other meshes and nodes in your model. This is a huge benefit, greatly simplifying the use of plate elements. It is not without drawbacks however. Here are some reasons why you might want to use manually created plate meshes.
Meshed Plate Limitations
- Auto meshes can be "ugly". If you have basically a rectangular area to mesh, you might just draw a single plate element and then split it into a very nice rectangular mesh! This will automatically split bordering members, but will not automatically connect to members passing-through the plate (out of plane), nodes falling on the interior of the plate area, or allow you to easily refine the mesh.
- There is currently no way to support an entire edge for an automatically generated plate mesh. You can insert some nodes along the boundary and support them manually, but the mesh generator may insert additional nodes between your supports and these nodes will not be supported, leading to "approximation errors".
- There is currently no way to provide spring supports under an automatically generated foundation slab mesh.
Convert to Manual Plates
Fortunately, you can take advantage of automatic meshing and then, when necessary "convert" an automatic mesh into manual plate elements. Then you can deal with the above situations. Of course, once you do this, you lose the management ability of the automatic mesh.
The finite element plate in VisualAnalysis is a "thin", flat numerical FEA device. It does not necessarily represent the things we have to model in the "real world". How do you model the following complexities with plates? The answer depends a lot on questions like:
- How much time do you have?
- What answers are you trying to get from the model?
- How accurate does your model need to be?
- Can you account for complexities in other ways, such as design checks or rules of thumb?
Composite Systems, Wood Shear Walls, Masonry
Concrete walls or slabs are reinforced (we generally ignore this reinforcement during analysis), and will crack, for example. Masonry systems have multiple materials and hollows. Wood shear walls consist of OSB panels with internal studs connected with unknown nail-patterns: these are true "beasts" with orthotropic materials and nail-slip! Good luck capturing that with a plate element. Modeling these kinds of systems will usually require you to make some serious assumptions. Normally in a VisualAnalysis model, these things are providing general stiffness to an overall frame and you are looking for how the forces distribute to beams, columns and foundations--not in the specific stress inside a 2x4 in a stud wall. Once you determine the wall force you can then go and design your wall using some other tool or procedure.
Stiffened Plates & Corrugated Metal Deck
These are a bit easier to deal with than concrete, masonry or wood systems. At least they are generally a single material. The organization of stiffeners or corrugation causes the entire panel or system to behave in an orthotropic way, which you may (or may not) need to capture in the model. You can sometimes get away with distributing loads from such a panel in a one-way fashion. In other cases you may need to use other devices such as creating perpendicular 'rib' plates in your plate mesh, or thickening plate elements along the lines of the ribs, or using member elements in the mesh to provide additional 'directional' stiffness. It all depends on what you are trying to learn from the model.