There are two methods available for designing reinforced concrete slabs in SPACE GASS:
With this method you define plate strips in the critical locations throughout your slab. Each strip is then designed for flexure, shear, torsion and deflection. The strips can be orientated in any direction with any desired width. Strips in different directions can cross over without affecting each other. You can display bending moment, shear force and torsion diagrams along the strips so that you can easily see which moments, shears and torsions the design is based on. Torsion is taken into account by adjusting the cross section moments using the Wood-Armer method Punching shear is a separate check that can be performed as described below.
Finite element method
The finite element method considers the moments throughout the slab and designs the flexural reinforcement on an element-by-element basis. Torsion can be taken into account by adjusting the x and y moments using the Wood-Armer method. Transverse shear is not considered in this method, however punching shear is a separate check that can be performed as described below. The results can be presented as a contour diagram for x or y reinforcement in the top and bottom of the slab or you can query any element to show the reinforcement calculations.
One advantage of the finite element method over the plate strip method is that it requires minimal input from the user and gives a fast overall design of the slab reinforcement, however it only calculates areas of steel and doesn't fit actual bars or mesh.
Cover and ductility
Both methods should give similar results, however the different treatment of cover and ductility in the two methods could cause different results in some circumstances. The differences are due to the fact that the strip method selects bars and/or mesh with known properties and dimensions from a reinforcement library, whereas the finite element method just calculates areas of steel. Cover in the strip method is measured as the clear distance from the edge of the outermost bars, mesh or stirrups to the edge of the concrete, whereas cover in the finite element method is measured to the centroid of the reinforcement. Ductility in the strip method is known based on the bars or mesh selected, however the finite element assumes normal ductility reinforcement with a capacity reduction factor of 0.8. If you are using low ductility reinforcement in the finite element method then you could manually increase the calculated areas of steel in proportion to the ratio of the normal and low ductility capacity reduction factors.
Punching shear is a separate check that is independent of the strip or finite element methods. Punching shear perimeters and utilization ratios can be shown graphically for the slab at each column-slab intersection or you can query the punching shear calculations. For more information refer to "Punching shear".
In order to use any of the above design methods you must have modelled your slab using plate elements. Of course your model can also include non-plate members for modelling beams, columns, braces, etc. that are connected to the slab. You must also ensure that your plate elements are properly meshed, usually with a finer mesh over supports, near voids and along edges compared to the mid-span areas of the slab. The mesh tools in SPACE GASS let you do this easily when you first create the slab or refine the mesh in particular areas later if required.
Drop panels or beams underneath the slab can
be incorporated into the slab design by the use of thicker plate elements
that have been offset downwards so that their top surfaces line up with
the top of the slab. The slab design would then consider them as a combined
T or inverted L cross section. If you model beams underneath with separate
members instead of using thicker plate elements then the analysis will
correctly allow for the interaction between the members and the plate
elements, however the slab design and the beam design would have to be
done separately. Modelling the beams and slab separately would also introduce
other complications because the bending moment in the combined section
is not just the sum of the beam and slab moments but must also take into
account the axial forces in the beam and slab and their distance apart.
Modelling drop panels or beams underneath the slab using thicker plate
elements is therefore the recommended approach.
The local axes of all the plate elements in your slab should be aligned so that any contour diagrams (and in particular reinforcement contours) are based on the same direction throughout the slab. If your plate axes aren't aligned then different parts of a contour diagram will be for different directions. When you use any of the mesh tools they automatically align all the axes for the plate elements that are generated, however the "Align plate axes" tool can be used to do this later if required. You can also use this tool to change the direction of all the plate axes in your slab to match the desired direction of your reinforcement.
A "Pattern loading" tool is available that recognizes regions defined by gridlines and loads them with a primary load case for each region. Combination load cases are also created that consider all adjacent and alternate span combinations of the loaded regions.
A linear analysis is more than adequate for carrying out a slab design/check at the ultimate limit state. A non-linear analysis can also be used, however due to the absence of any significant p-delta effects in slabs, the design actions are likely to be similar to those from a linear analysis. Note that the plate elements in SPACE GASS are linear elements and will therefore behave linearly even if a non-linear analysis is performed. Note also that a non-linear analysis does not include any material non-linearities and assumes a linear stress-strain curve.
Deflections and cracked section properties
The strip method calculates deflections based on cracked section properties even if gross properties are used in the analysis. They can be displayed for each strip by clicking the "Deflections" tab in the slab strip editor.
Deflections for the finite element method are based purely on the section properties used in the analysis. They are displayed as standard contour diagrams and/or deflected shapes by selecting the "Show displacements" or "Show plate contours" buttons on the side toolbar. You can view or change the section properties of a plate by double-clicking it and referring to its "Thickness" properties in the data panel that appears. Alternatively, you can access the section properties for multiple plates by selecting them individually or via a selection window, right-clicking and then selecting "View/Edit Plate Properties (Form)" from the popup menu that appears. For example, if you wanted the analysis of a 200mm thick slab to be based on a cracked moment of inertia of 0.4Ig instead of Ig then you would need to set the "Bending" thickness of the plate elements to 200*0.41/3 = 147mm. Note that a bending thickness of zero is interpreted as being equal to the actual thickness. Keep in mind that changing the bending thickness not only affects the deflections but also the bending moments and shear forces to some extent.
A "Span-to-depth calculator" tool is also available that calculates a slab depth that satisfies deflection criteria based on suitable L/d rules from the design code.
The concrete slab design module may also be used to design raft footings. For further information refer to "Concrete footing design".
A video showing the reinforced concrete slab design module in action can be viewed at www.spacegass.com/rcslab.
Note that if you haven't purchased the concrete slab design module, you can still run it in a free trial mode that limits you to using a predefined slab thickness, and prevents you from exporting or saving the job. All other features are fully activated.
Refer to the following sections in this chapter for full details of the concrete slab design module.