StructuralModellingManual_Arup.pdf

Structural Guidance Note 3.5a Structural Modelling Manual

STRUCTURAL GUIDANCE NOTE 3.5 REV A STRUCTURAL MODELLING MANUAL CONTENTS 1

Introduction

2 2.1 2.2 2.3

Modelling principles The Aims of Structural Analysis Modelling procedure Selecting the Model and its Properties Scheme design models, Final analysis models Preliminary Hand Analysis Computer analysis Checking the results Using the results

2.4 2.5 2.6 2.7 3 3.1 3.2

3.3

3.4

Modelling Specific Structural Members General Considerations Beams and Columns General Principles, Members of uniform straight cross section, Members of non uniform straight section, Perforated members, Curved members Joints and connections between beams and columns General Principles, Joints in Concrete frames, Joints in steel frames, Joints in other materials Slabs and Walls General, Floor slabs in large building models, Suspended floor slab analysis - flat slabs, Suspended floor slab analysis - beam and slab, Shear walls in large models , Shear wall analysis, Basement floor slab analysis flat slab, Basement Floor Slab analysis - beam and slab, Plate and shell structures

4 4.1 4.2 4.3 4.4 4.5 4.6

Modelling Specific Structure Types Multistorey buildings Roof structures Symmetrical structures Tunnels and culverts Cylindrical structures Bridge decks

5

Member section properties General, Cross Sectional Area (A) and Shear factors (Ky, Kz), Flexural Second Moment of Area (Iyy, Izz), Torsional Second Moment of Area (J)

6 6.1 6.2

Material properties General Reinforced Concrete Properties for ultimate strength analysis, Properties for serviceability analysis, Properties for dynamic analysis Steel Composite Timber Other materials Wrought Iron, Cast Iron, Masonry, Aluminium

6.3 6.4 6.5 6.6

1/44

April 03


7 7.1 7.2 7.3

Modelling Loads General Point of application of load Self weight

7.4

Other permanent loads

7.5

Transient loads

7.6

Internal loads Temperature, Lack of fit, Prestress, Support settlement

8

Modelling restraints General, Restraint at ground, Raft Foundations, Global restraints, Support settlement

9

Modelling for dynamic analysis

10 10.1 10.2

Interpretation of results Beams and columns Slabs and walls

11 11.1 11.2 11.3 11.4 11.5 11.6 11.7 11.8 11.9 11.10 11.11 11.12 11.13 11.14 11.15 11.16 11.17 11.18 11.19

Additional Information Warnings and errors during analysis Concrete post processing of 2D element results P-delta effects Modelling castellated beams, trusses etc. by shear beams Modelling beams with long slabs Grillage analogy for slabs Setting up a model with 2-D elements Axis systems and element orientation Section properties for standard shapes Multi storey frame models Modelling bridge decks Section properties from first principles Modelling haunched beams Modelling elements with rigid ends Modelling beams and slab floors with in plane stresses Symmetrical & anti-symmetrical loads Equivalent loads for pre-stressing Properties of standard materials Holes in reinforced concrete beams

12

Revision History

2/44

April 03


1 INTRODUCTION This note gives guidance on the representation of a real structure by an idealised model which can then be analysed. 2 MODELLING PRINCIPLES 2.1 The Aims of Structural Analysis Analysis is an essential part of the structural design process. Analysis gives us the numbers with which to justify the adequacy of the structure in terms of strength, stability and stiffness. However we do not analyse 'the structure' but a mathematical model whose properties and behaviour we aim to select so that it adequately represents the real structure. The approximations and assumptions which must be made to create this model mean there can be no such thing as an exact model.

There is a commonly held belief that present day analysis is necessarily more 'accurate' than earlier methods were. However, while results of computer analysis are 'precise', unless the analytical model is carefully chosen the results may be misleading and could be dangerously wrong. Before embarking on an analysis it is necessary to consider what analysis is needed: • What needs to be demonstrated, what will dictate the design? Eg strength, deflection, stability • What is the simplest model which can demonstrate this? The simplest model will be the easiest to understand, the quickest to set up and use and so probably the most cost effective • What effects will be ignored or misrepresented by this model? Are they significant? Eg the analysis will normally assume linear elastic materials and small deflections. • What results will be produced? Can they be used to demonstrate the desired effect? Eg 2D element analysis produces stresses which may not be easy to convert into design forces and moments. • What will happen to the reactions from this model? Eg Can the foundations resist the forces generated?

3/44

April 03


2.2 Modelling procedure There are a number of steps in the production and analysis of a mathematical model of a structure. Engineering judgement is needed throughout the process, and the modelling decisions made should be reviewed as part of the design review. • Decide how much of the structure to model. (section 2.3) • Decide how much detail is needed in the model. This will depend on whether the model is for scheme design or final analysis . (section 2.3) • Define geometry of model Define member sizes and shapes (section 5) • Decide on appropriate material properties (section 6) Define loading to be applied • Decide how to apply the load (section 7) Analyse the model • Review analysis results (section 2.6) 2.3 Selecting the Model and its Properties Scheme design models The model needed for a quick scheme design can usually be very much simpler than the model used for final detailed design calculations, and in many cases hand calculations will be sufficient. The form of the structure is still evolving at this stage and fundamental parameters may need to be altered or varied to determine the most appropriate design. Issues which are not considered at this stage but which need to be investigated at a later stage, should be clearly identified for the final designer to pick up. Members derived from such simple models should be sized conservatively to allow for design development. Final analysis models Once the detailed structural geometry has been defined, use of a more complex model may be justified. The capacity of the latest generation of computer programs makes it possible to build very large and complex models but these can be counterproductive, because the volume of data may increase the chances of errors and makes it more difficult to pick them up. For many structures, analysis of simple sub frames will be adequate for final design. A structure should only be analysed as a three-dimensional model if the designer is satisfied that simpler models cannot adequately predict the behaviour. This remains true if a three-dimensional CAD model of the structure has been created. For further guidance on when a three-dimensional model is appropriate see multistorey buildings (section 4.1) 2.4 Preliminary Hand Analysis The engineer must be able to visualise how he or she expects the structure to work, and must have an idea of the magnitude and form of answers anticipated, before any analysis is done. A sketch of the expected deflected form and some simple hand calculations should always be done, however complex the model, to ensure that gross errors in modelling will be picked up.

4/44

April 03


2.5 Computer Analysis Most computer programs for structural analysis will carry out a linear elastic analysis, assume deflections are not large enough to affect the force distribution and assume that plane sections remain plane. The engineer must always remember that these assumptions are being made and consider whether they are appropriate to the structure being modelled. In structures where deflection would affect the forces in the structure, these effects need to be considered (P-delta effects section 11.3). The assumption that plane sections remain plane is not valid at complex joints and discontinuities and a more detailed analysis in such areas, using 2D elements, may be necessary. Walls, slabs and plates may be modelled using a grillage of skeletal elements, or by using 2D elements. Special structures (eg cable nets) or loadings (eg seismic) may require more complex models and/or analyses. Specialist advice should be sought before starting such analysis. Problems may be encountered during analysis which either prevent results being produced, or give warnings that the analysis may not be valid.(section 11.1) Input data should always be checked carefully. Some one who did not develop the model should check it. The analysis program's facilities for graphical representation of the data should be used to the full in checking. 2.6 Checking the results Always confirm that no warning messages were produced by the computer during the analysis. If warnings have been produced, their implications should be evaluated before proceeding further. See the program manual for guidance on this topic. Results should always be checked against the preliminary hand analysis. • Look at the deflected form of the structure under each basic loadcase, looking at the magnitude of peak deflections as well as the form. • Compare the sum of reactions for each basic loadcase with the applied load (to check for analysis errors like ill conditioning) and the total load on the model with the total load on the structure (to check for input errors). • If the model and loading is symmetrical, check the results are symmetrical. • Check the restraints are restraining the structure in the intended directions. • Compare bending moment, shear force, axial load and reaction plots from the computer analysis with the predictions. If the results do not correspond to the predictions the following procedure should be followed: • Check the input data again, graphically and line by line. • Check that elements are correctly orientated and relative stiffnesses are sensible. • Check that loading is correctly applied. • Seek advice from colleagues and/or specialists. • Review the modelling assumptions. • Review the hand analysis. Examination of the computer results may show trends which were not previously recognised, which can in turn lead to a radical reinterpretation of the behaviour of the structure. If after this the hand calculations and the computer results cannot be reconciled seek advice. Never accept the results of a computer analysis without an engineering explanation for the behaviour predicted by the computer. A number of expensive mistakes have been made in recent years by engineers who have ignored this rule.

5/44

April 03


2.7 Using the results Once the results have been checked and found to be reasonable they can be used for member design. The results from the analysis of a skeletal structure can often be used directly for design but most other results will need to be post-processed to derive forces which can be used in member design. (section 10) 3 MODELLING SPECIFIC STRUCTURAL MEMBERS 3.1 General Considerations Structures are generally made up of three types of member:

A beam or column, with a length which is large compared to its cross sectional dimensions.

A slab, wall or plate, with a thickness which is small compared to its length and breadth eg a concrete slab.

A solid, with significant dimensions in all three directions, eg a small deep pilecap.

Divisions between these categories are not always clear cut. Analytical models in a computer are made up of discrete, 'finite' elements, which are only connected together at their extremities (as opposed to the actual structure with its infinitesimal elements forming a continuum). Again these finite elements come in three types:

A one-dimensional element, defined by the position of its two ends and the properties of its cross section, connected at its ends only (a beam element).

A two dimensional element, defined by the position of its corners and a thickness, connected at its edges only (a plate or shell element).

A three dimensional element, defined by the position of its corners, connected at its faces (a brick element). This type of element is used in specialised structural analysis only and will not be considered further in this note.

The divisions between these types are clear-cut. A one-dimensional element is always represented mathematically by a line of zero cross section and a two dimensional element by a surface of zero thickness.

6/44

April 03


The selection of the appropriate idealised element to model specific members of real structures is described below . 3.2 Beams and Columns General Principles Generally these are the easiest members to represent in a model. There will be a simple correspondence between the member in the structure and the element in the model. Problems come at joints where the members meet (section 3.3), and where forces in the member are changed by deflection under load (P-delta effects section 11.3).

Members of uniform straight cross section Simple bending theory, assuming plane sections remain plane and neglecting shear deformations, gives an adequate model of beams with a span/depth ratio of 10 or more (for steel and concrete). A shear beam, which includes the effect of shear deformation, should be used for elements with a smaller span/depth ratio. Using shear beams for all elements will not increase the size of the problem for the program and so their use is recommended. It is generally assumed that only part of the cross section of a beam resists shear deformation (eg the

web of an I beam) and so the proportion of the cross section which is assumed to carry shear has to be defined, usually by a shear factor (section 5.2). Once the span/depth ratio is 2.5 or less a reinforced concrete beam should be designed as a deep beam in accordance with CIRIA Guide 2. Deep steel beams with a span/depth ratio of 1 or less are unlikely to behave as beams and should be stiffened to suit a strut and tie model.

7/44

April 03


Members of non uniform straight section

Haunched and tapered beams can be analysed by choosing a mean stiffness or by modelling different parts of the beam with different properties. (section 11.13) Perforated members

Isolated holes or recesses which extend over less than 5% of the length of the beam do not significantly affect its stiffness and can be ignored in analysis (but must be considered in design of the member). Local effects around holes need to be considered in design, detailed guidance for dealing with holes in reinforced concrete beams is given in section 11.19.

A member with a line of holes (for example a castellated beam), a truss or a Vierendeel girder can be modelled as a single shear beam. (section 11.4)

8/44

April 03


Larger holes and long slots should be represented in the model by splitting the member into sections. (section 11.5) Curved members

A curved member may be modelled as a series of straights. Generally the angle between successive elements modelling a circular arc should not exceed 15 degrees. The curve introduces additional forces into the member which are not modelled by the series of straights. To include for these effects within the model, each member between intersections with other members needs to be modelled by at least two elements (or more if necessary to satisfy the 15 degree rule given above). The additional node should be placed at the point of maximum deviation of the curve from the straight line joining the ends. 3.3 Joints and connections between beams and columns General Principles One-dimensional elements in a model have zero cross section and so they meet at a point. The connection at this idealised point in the model can be one of two types: • A rigid joint, in which there is no relative rotation between elements meeting at a point. • A pinned joint, in which no moment is transferred between elements meeting at a joint. A partially fixed joint, where a rotational spring is used to transfer moment across a joint while allowing some rotation, could be included in a model but the value to be used for the spring stiffness is uncertain. If the analysis is sensitive to joint stiffness, then analysing for both a fully fixed and fully pinned condition, and designing for the worst case in each element is recommended for strength design. Because real members are not of zero thickness, they never meet at a point. True pins are rare, unless a proprietary bearing is used. Truly rigid joints never occur, although many joints are stiff enough for the difference to be neglected. Joints in steel structures (section 3.3.3) even when apparently stiff are usually modelled as pinned which simplifies joint design and ensures that members designed to resist sway carry all horizontal loads. Where a nominally pinned joint has to be able to rotate (for example at the end of a long 'simply supported' truss) the capacity of the actual connection to accommodate those rotations must be checked.

9/44

April 03


Joints in Concrete frames

Joints in monolithic concrete frames should normally be modelled as rigid. It is unrealistic to model any monolithic joint as pinned, and reinforcement must be provided to limit cracking in all such cases. If in a subframe analysis a beam is assumed to be pinned to the columns then column moments will need to be calculated separately. A better solution is to model the columns as part of the subframe. Finite Joints Where the members intersecting at an idealised joint have substantially different flexural stiffnesses, the stiffer members will restrain the flexure of the other members. These flexible members can be modelled using a single element with a transformed stiffness, or an element with rigid ends. (section 11.14)

Large joints can be analysed using 2D elements to determine the distribution of stresses and to give a better estimate of stiffness of the joint. Note that the dilation of 2D elements under axial load is restrained by rigid constraints and supports (which are a convenient way to apply loads from a beam analysis to such models), giving some unexpected and normally spurious stresses local to the constraint.

10/44

April 03


Joints in steel frames

The cost of joints between members in a steel structure is a large proportion of the total cost. It is therefore desirable, wherever possible, to use simple design methods, assuming pinned connections. In triangulated structures (trusses) rotations at joints are usually small and so even welded joints can be considered as pinned. Joint fixity is needed for stability in the design of moment frames and portals and should normally be assumed when a steel member is continuous through a joint. Haunched joints in portals need to be modelled by more than just a beam and column meeting at a point.

At the end of a steel truss, where a number of steel members meet at 'a point', it would be normal to join the diagonal bracing member to the beam before the beam is joined to the column. The beam to column connection will therefore need to be designed for the resultant of the forces in the beam and diagonal, not just for the end forces in the beam as derived from the analysis. There are often situations where it is not appropriate for the centrelines of members to meet at a point and generally the resulting eccentricity needs to be modelled. EC3 annex K.3 allows small eccentricities to be ignored (the eccentricity has to be less than between 0.25 and .55 times the main member depth, depending on the arrangement of the joint) Joints in other materials Joints in timber Achieving a rigid joint in timber construction is very difficult, so joints should generally be modelled as pinned. Connections are often eccentric and the moments generated by this and by partial fixity need to be considered in design.

11/44

April 03


Joints in masonry Unreinforced masonry joints cannot take tension. Unreinforced masonry should not generally be analysed in a linear elastic program. 3.4 Slabs and Walls 3.4.1 General The modelling of slabs and walls is more complicated than the modelling of beams and columns. There are often several different ways in which a given member can be modelled and the best model to use will depend on a number of factors: • Is it subject to in-plane forces, out of plane forces, or a combination? • Is it a uniform isotropic material? (reinforced concrete isn’t) If not can the results be manipulated to give useable design forces? • Is it to be modelled on its own or as part of a larger model? • On its own: Is it a simple, regular structure that can be designed using simple rules, without computer modelling? Are there holes or discontinuities that will lead to stress concentrations? • As part of a larger model: Are forces within the slab or wall of interest in this model, or just its effect on the surrounding members? To illustrate the approach to modelling slabs and walls the following sections show how these factors influence the selection of models for some common structural members. 3.4.2 Floor slabs in large building models Where a large irregular building consists entirely of sway frames, a 3D skeletal model is often appropriate (but not for buildings with stability cores section 4.1). Floor slabs in such buildings will generally be very stiff in plane compared to the columns (except at the base of tall buildings where columns are likely to be very stiff ) and axial forces in the slabs are generally neglected in slab design. The simplest way to represent the high in plane stiffness of such slabs in the model is to link the nodes attached to the slab rigidly together at each level to prevent relative in-plane movement. If the model is to be used to investigate shrinkage, prestress or temperature effects then a rigid link cannot be used. A mesh of 2D elements or a grillage of beams could be used to model the slab but these effects would normally only be investigated in local element models of either a flat slab (section 3.4.3) or a beam and slab deck (section 3.4.4). 3.4.3 Suspended floor slab analysis - flat slabs Simple methods of analysing regular flat slabs, including coffered slabs, spanning in one or two directions are described in BS8110 (and EC2) and more details are given in CIRIA Report 110. These methods should generally be used where possible. In-plane stresses in suspended slabs, for example those generated as horizontal wind loads are transferred from the facade into the stability cores, are generally neglected in analysis. However prop forces from retaining walls on basement slabs (section 3.4.7) may need to be considered. If supports are not in a regular pattern then analysis under out of plane loading only can be carried out by representing the slab as either a grillage of skeletal elements or a mesh of 2D plate bending 12/44

April 03


elements. Note that coffered slabs need to be modelled in such analysis as beam and slab decks( section 3.4.4). Defining the element properties for grillage analysis (section 11.6) is more difficult but the 2D element mesh (section 11.7) needs to be set up carefully to ensure adequate results. Interpreting the results of the 2D element analysis is more difficult, unless a post processor (section 11.2) is available to convert stresses into areas of reinforcement. Guidance on setting up a grillage model for a flat slab is given in CIRIA Report 110.

Cracking of concrete close to supports leads to significant redistribution of moment away from the support. This reduction in stiffness (EI) can be modelled by reducing E in the analysis. Iteration to refine the extent of cracking is likely to be necessary. Note that this is effectively a non linear analysis, and so must be done for the appropriate loadcase, since superposition of loadcases is not applicable. Sharp peaks of moment/stress at internal supports derived from analysis may be averaged, as in a hand analysis, over half the column strip width. If there are large voids in such slabs the modelling round these holes needs to be considered carefully. Checks for punching shear close to supports or concentrated loads should be done by hand, not by trying to refine the analytical model of the whole slab. 3.4.4 Suspended floor slab analysis - beam and slab Simple rules for analysing ribbed slabs (one way spanning) and coffered slabs (two way spanning) are described in BS8110 (and EC2) and these should generally be used where possible. In-plane stresses are generally neglected in analysis. However prop forces from retaining walls on basement slabs (section 3.4.8) may need to be considered. If supports are not in a regular pattern then analysis under out of plane loading only can be carried out by representing the slab as a grillage (section 11.6) of skeletal elements. 2D element analysis of ribbed or coffered slabs is not recommended.

13/44

April 03


If there are large voids in such slabs the modelling round these holes needs to be considered carefully. Checks for punching shear close to supports or concentrated loads should be done by hand, not by trying to refine the analytical model of the whole slab. 3.4.5 Shear walls in large models Where a shear wall is to be included in the model of a large building (section 11.10) it will often be sufficient to model it as a vertical 1D element. Rigid links, or rigid ended elements (section 11.14), can then be used to join the point where horizontal elements intersect the edge of the wall to the 1D element representing the wall. 3.4.6 Shear wall analysis

If a shear wall has a complex shape, with voids in different places on different floors, a 2D element plane stress analysis should be done to identify stress concentrations round the voids. Out of plane bending of shear walls is normally neglected, because there is other structure perpendicular to the wall which will resist this bending. If this is not the case a general 2D element model, which can carry both in plane and out of plane moments, can be used. Setting up the 2D element mesh needs to be done carefully to ensure adequate results, particularly at corners of holes (section 11.7). The mesh illustrated above has been refined in these areas to achieve this. Interpretation of the results of this analysis into required areas of reinforcement is complicated and the use of a post processor is recommended (section 11.2). 3.4.7 Basement floor slab analysis - flat slab Both in plane forces from surrounding retaining walls and out of plane forces from vertical load, are often significant in the design of basement floor slabs. Where the geometry of such slabs is complex, a model using general 2D elements able to resist in plane and out of plane forces can be used. If beam strips across the slab can be identified then a space frame skeletal model (a grillage able to accept in plane and out of plane loading) can be easier to use.

14/44

April 03


Setting up the 2D element mesh needs to be done carefully to ensure adequate results (section 11.7). Interpretation of results of this analysis into required areas of reinforcement is complicated, because the principal stresses in the element will not normally line up with the reinforcement directions (section 11.2). 3.4.8 Basement Floor Slab analysis - beam and slab Where a basement floor slab has ribs, beams, or coffers it can not be represented adequately by a mesh of 2D elements alone. A grillage of beams gives a good model of out of plane effects and is not very inaccurate in modelling the in plane strains in a regular slab. A mixture of beam and 2D elements gives the best model of the behaviour of this sort of floor but interpreting the results from such a model is very difficult. More details of the options available are given in section 11.15. 3.4.9 Plate and shell structures General 2D elements can be used to approximate curved surfaces from a series of flat elements. These structures can then be loaded in any direction. The mesh needs to be fine to limit the angle between adjacent elements. Specialist advice on modelling curved shells should generally be sought. Setting up the 2D element mesh needs to be done carefully to ensure adequate results.(section 11.7) For steel shells the resultant stresses can be used directly for design, provided the effects of buckling and shear lag (reducing effective widths) are considered in the design. For concrete shells, interpretation of the results of this analysis into required areas of reinforcement is complicated and the use of a post processor is recommended (section 11.2).

4 MODELLING SPECIFIC STRUCTURE TYPES 4.1 Multistorey buildings For many structures, where lateral stability is provided by stiff cores, simple sub frame models each containing a single beam and the columns above and below it, will be adequate for the analysis of concrete structures and simple hand analysis for steel structures. With very unequal spans the difference in axial loads in adjacent columns can make a subframe analysis inappropriate (because the heavily loaded column is compressed more). Columns need to be checked at near the top of the building where bending dominates and axial loads are small. The cores can then be modelled as plane frames resisting the full lateral load in two orthogonal directions. Using a three dimensional model of the full building in such cases is not recommended. It would not only be far more complicated to set up and check but would also imply that the whole structure

15/44

April 03


forms part of the lateral load resisting system. Changes to the secondary elements during design development or later refurbishment would require re-analysis. For structures where a three dimensional analysis is needed, various techniques for generating both simple and complex models have been developed (section 11.10). 4.2 Roof structures If a roof structure consists of identical primary frames in one direction, supporting purlins spanning between them, there is no advantage in modelling the whole structure. A plane frame model of the primary frame will be adequate. Sometimes however frames have different stiffnesses or pick up different loads and support a continuous secondary structure, stiff enough to transfer loads between the frames. Determining the distribution of loads between these frames to apply to a series of plane frames, ensuring compatibility of deflections, would then be complex and iterative. A space frame model which does this automatically is appropriate. 4.3 Symmetrical structures If a structure is symmetrical, then only a half or a quarter of the structure needs to be modelled. However the additional complexity introduced by having to set up different models for antisymmetric and symmetric loads means that this should only be considered if the full model is too big for the computer to analyse. Details of the restraint conditions needed on the axes of symmetry and splitting loads into symmetric and anti-symmetric components are given in section 11.16. 4.4 Tunnels and culverts

Structures with constant cross section over a long distance, without joints and loaded uniformly and in the plane of the cross section only, can be analysed using 2 dimensional elements in a plane strain analysis (not to be confused with a plane stress analysis section 3.4.3). However effects close to joints, local loads and hard points tend to govern such designs, and plane strain analysis is not appropriate in these areas. Soil structure interaction is also likely to dominate design of tunnels and specialist advice should be obtained on how to model this.

16/44

April 03


4.5 Cylindrical structures

Cylindrical tanks and other structures where the loading and structure are symmetrical about an axis of rotation, can be analysed using two dimensional elements in an axisymmetric analysis. Any departure from symmetry (a wall attached to the side of the tank for example) will invalidate the analysis. 4.6 Bridge decks Bridge decks, unlike buildings, tend to be long span isolated structures. The way these decks are modelled will depend on the form of the deck. Guidance on the modelling of bridge decks (section 11.11) is given in ‘Bridge Deck Behaviour’ by E.C, Hambly (Spon, 1991)

5 MEMBER SECTION PROPERTIES General This section describes the derivation of properties for given shapes of member, assuming they are formed from uniform linear elastic materials. If the material being used is a composite (eg reinforced concrete) these properties will need to be modified (section 6). Most computer programs will generate the properties required by the analysis from the dimensions of the cross section for standard sections and this facility should be used where possible. Certain parameters for unsymmetrical standard sections cannot be generated automatically because they depend on the end connections. Note that modelling an angle or channel section taking any bending, torsion, or shear is very complicated because the shear centre is outside the section. Properties for irregular sections may need to be derived by the user.

17/44

April 03


Beams and columns have a cross section which can be defined geometrically and this section has properties which can be derived from those dimensions. Which properties need to be defined depends on the type of analysis. The full range of properties (as needed for a 3D space frame structure) are detailed below.

The properties are defined relative to a local axis system for the element (section 11.8). Details of this system will be given in the computer program manual, generally the local x axis is along the length of the element and the y and z axes should be the principal axes of the cross section. Slabs and walls modelled by 2D elements have a thickness only and no further geometric properties need to be defined. Slabs modelled by 1D elements in a grillage are covered in section 11.6 In a linear elastic analysis the reduction of stiffness in compression of slender members due to buckling is ignored. It is possible to do an iterative analysis of a structure incorporating tie bars (which can be assumed to take only tension and buckle under compression) by reducing the stiffness of any tie elements which are found to be in compression, but a non linear analysis may be more appropriate. Specialist advice should always be sought before carrying out such an analysis. Cross Sectional Area (A) and Shear factors (Ky, Kz) The area used for axial stiffness and stress calculations will generally be the cross sectional area (‘ the concrete section’ ignoring reinforcement in BS8110). The net area of members perforated by a series of holes should be used. The area used for shear stiffness calculations will generally be less than the cross sectional area. It is usually defined by a shear factor, which is the proportion of the total area which is assumed to carry shear (e.g. the web of an I beam). Shear factors for various shapes are derived in Structures Note 1992NST_21. Flexural Second Moment of Area (Iyy, Izz) The I value used for bending stiffness can be calculated from first principles (section 11.12), and is tabulated for most rolled sections in published data sheets, and for simple shapes in publications like the Steel Designers Handbook. Note that most sections have significantly different I values in the two orthogonal directions and so the orientation should always be checked visually in the model. Torsional Second Moment of Area (J) Calculation of the torsion constant (J) used for torsional stiffness is an area of modelling where the rules to be applied are complex and the appropriate value to use depends on end conditions as well as the cross section. Methods of deriving J for commonly occurring shapes are given in section 18/44

April 03


11.12. Note that, except for circular cross sections, the torsion constant is not the polar moment of inertia (which can be calculated from first principles). For a flat slab modelled as a grillage (section 11.6) the torsional stiffness GJ should equal the bending stiffness EI. In some structures all torsion constants could be set to zero without significantly affecting the results. This cannot be done in any structure that relies on torsion to carry the load, such as an eccentrically loaded beam. Torsional stiffness must not be neglected in torsionally stiff structures such as box sections. The effect of warping, particularly on open ended box girders, can significantly reduce the apparent torsional stiffness of such members. Remember that if torsional stiffness has been included in a model then the torsions derived from the analysis must be considered in the member design. Simple rules for combining torsions and bending moments in a grillage are given in Structures Note 1991NST_16. 6 MATERIAL PROPERTIES 6.1 General The material properties of a uniform linear elastic material can all be derived from the elastic modulus, E, (also known as Young's Modulus) and Poisson's Ratio, ν. Values for these two parameters are tabulated along with the density and coefficient of thermal expansion, for common construction materials in section 11.18 Because real materials are not uniform, or elastic, some modifications to material or section properties need to be made, as described below. 6.2 Reinforced Concrete Reinforced concrete is a composite, made up of two very different materials. Reinforcing steel can be assumed to be a linear elastic material for the purposes of analysis but the concrete matrix has a very different stiffness, is subject to shrinkage and creep and cracks under tension. Simple rules given in design codes allow the use of ‘the concrete section’ (ignoring reinforcement), ‘the gross section’ (including all the concrete and the transformed reinforcement) or ‘the transformed section’ (including concrete in the compression zone only plus the transformed reinforcement). Differences between these values can be significant and the designer needs to consider which is appropriate. Properties for ultimate strength analysis Most analysis of concrete structures is concerned with deriving forces for ultimate strength design and so is not usually sensitive to the absolute stiffness value assumed. Only if the model contains a mixture of steel and concrete members, or members made from concretes with significantly different stiffnesses (>15%), or the axial stiffness of columns is important, for example in tall buildings, will the absolute stiffness of the concrete be important. If absolute stiffness is not critical, the non linear and composite nature of concrete can be ignored and the standard material properties (section 11.18) can be used with the concrete section dimensions. Special rules apply to a flat slab modelled as a grillage (section 11.6). Halving the torsion constant of any solid concrete member (where this is included in the strength analysis section 5.4) to allow for cracking of the section is a reasonable simplification. Properties for serviceability analysis In standard construction, deflection under service loads is generally covered by limiting span/depth ratios, and cracking is covered by detailing rules. In this case a serviceability analysis is not normally required. 19/44

April 03


If a serviceability analysis is required then more care needs to be taken with the definition of stiffness. The results obtained from this analysis are unlikely to be accurate and the possibility that deflections will be significantly larger or smaller than the calculated value must always be remembered. The following matters need to be considered in these exceptional cases to determine the most appropriate values for material and geometrical properties to use: Creep If a concrete member is subject to sustained loading it is observed that the deflection increases over time. The amount of this increase, known as creep, is sensitive to the time after casting at which the concrete is loaded, the humidity of the atmosphere, concrete mix, member size and subsequent loading history. The effects of these factors on the degree of creep is defined in the codes of practice for concrete and is allowed for by modifying the short term elastic modulus by a creep factor. Note that E is modified by 1/(creep factor + 1). If a serviceability analysis is being carried out it will not normally be sufficient to accept default values for ‘long term E’. Shrinkage Unrestrained concrete shrinks with time. Shrinkage needs to be considered in calculating losses in prestressed concrete. In very large slabs without movement joints and with stiff external restraints the tensile forces generated by restraint to shrinkage may need to be considered. In a frame analysis program the effect of shrinkage is entered by specifiying an initial strain on the element or, if this feature is not available, by specifying a temperature change which will give the equivalent strain. Reinforcement Because reinforcing steel is much stiffer than the concrete matrix the uncracked composite material will be stiffer than an unreinforced concrete section of equivalent size. It is possible to allow for this by calculating the geometrical properties of a transformed section, where the area of reinforcement is multiplied by the modular ratio (Esteel/Econcrete-1). If this is done then the effects of cracking, which reduces stiffness, must also be considered, see below.

Note that axial load in columns increases the area in compression, and so the effect of cracking in columns will generally be less than in beams. Note that the value of Econcrete used to determine the transformed section properties will depend on whether creep effects are being considered. The value used to calculate the section properties should also be used when defining the material properties. Cracking Once part of a concrete member goes into tension, it is likely to crack and the stiffness will then be reduced. Because the amount of cracking depends on the loads applied, the stiffness of the member 20/44

April 03


will vary with load. This cannot be allowed for in a linear elastic analysis and so, if the most accurate estimate of deflection possible is needed, an iterative analysis is required, reducing the element stiffnesses where an initial analysis of uncracked sections shows that cracking would occur. Stiffness of cracked sections in this case needs to be determined from the moment-curvature relationship for the section. Note that it is the stiffness (EI) which needs to be adjusted, and in many cases (including all 2D element analysis) it is easier to modify E to allow for these effects, instead of changing I (or the section dimensions from which I is calculated). Properties for dynamic analysis Stiffness is important for dynamic analysis and so cracking and reinforcement may need to be considered, as for a deflection analysis. If loading is applied rapidly to concrete it is stiffer than when load is applied gradually. The increase in stiffness is of the order of 10% for earthquake or extreme wind loading and so is generally neglected. Larger increases in stiffness are observed with low amplitude dynamic loads, in vibration analysis of floor slabs for example. Further details are given in 'An Arup Introduction to Structural Dynamics' by Mike Willford. 6.3 Steel Most structural steels can be assumed to behave in a linear, elastic manner up to yield and then to deform indefinitely at that level of stress, forming a plastic hinge. Analysis of models including plastic hinges is non linear and outside the scope of this note. For further details on the use of plastic theory, see Plastic Design to BS5950 by J.M. Davies and B.A. Brown, Blackwell, 1996. 6.4 Composite (steel beam and concrete slab) Properties for analysis in sagging regions need to be calculated for a transformed section, allowing for the different modulus of steel and concrete, usually by reducing the effective width of the slab in the ratio Econcrete/Esteel. Note that in hogging regions the concrete slab will be cracked and will not therefore contribute significantly to the stiffness of the composite beam. Rules for the proportion of the span to be taken as cracked are given in design codes. As with concrete structures the effects of creep on the stiffness of the concrete need to be considered. 6.5 Timber Timber, as a natural material, has a wider variation in stiffness than manufactured materials. Mean and minimum values of E are given in the codes. Generally the minimum stiffness value should be used in a frame analysis and the mean stiffness should only be used where significant load sharing between members is possible (e.g. floor joists). The effect of timber being stiffer than assumed may need to be considered. 6.6 Other materials Typical properties for the materials described below are tabulated (section 11.18) but the following points need to be considered when modelling these materials: Wrought Iron Wrought iron behaves in a similar manner to steel. Further details are given in The Appraisal of Existing Iron and Steel Structures. (SCI publication 138)

21/44

April 03


Cast Iron Cast iron is not a linear elastic material. Stiffness reduces as load increases and the tension stiffness is less than the compression stiffness. Brittle failure under tension occurs at comparatively low stresses. Providing these features are born in mind a linear elastic analysis can give reasonable results to use in strength design. For deflection calculation a range of stiffnesses would need to be considered. . Further details are given in The Appraisal of Existing Iron and Steel Structures. (SCI publication 138) Masonry Masonry is assumed to crack at the joints under tension and so the stiffness of a masonry element will reduce once the extreme fibre goes into tension. Aluminium Aluminium can be treated as a linear elastic material for analysis. Designers should be aware that there will be significant reduction in strength of the material at any welded connection and this lower strength will need to be used in design. 7 MODELLING LOADS 7.1 General It is usually convenient to split the load into a number of loadcases which can then be combined with appropriate load factors. 7.2 Point of application of load If only part of a structure is modelled, it may not be possible to apply loads to the model at the same position as they are applied to the structure. Care is needed to ensure that the eccentricity of load is considered in this case, particularly for cantilevers. Sometimes local effects of loading are calculated separately (e.g. wheel load effects on a bridge deck) and only the global effects are to be determined from the model. In this case it is important that loads are applied to the model on the primary structure, with any moments resulting from the eccentricity of loading. Otherwise the results from the global analysis will contain a local component which will therefore be included twice in the total analysis. 7.3 Self weight It is possible in many programs to have the self weight calculated automatically from the areas of the elements and the density of the materials. A number of issues need to be handled carefully if this approach is adopted: • When modelling a slab using a grillage, this approach will apply twice the total weight of the slab, unless special precautions are taken (e.g. using two different materials, one with a density of zero, for longitudinal and transverse elements). • Additional load from stiffeners, connections etc will not be included. • Dummy elements with arbitrary large cross section will generate large loads. Mixing gravity loads and applied loads in a single loadcase is not recommended, because checking of loading will be complicated and, especially if any of the problems noted above are present, the use of applied loads to represent the self weight is generally preferable.

22/44

April 03


7.4 Other permanent loads Generally other permanent loads will be present in addition to the self weight of the members and these loads have to be applied explicitly to the model. It is generally best to apply the load to the model in a similar manner to the way in which loads are applied to the part of the structure which has been modelled (e.g. on a plane frame: apply purlin loads as point loads, slab loads as distributed loads). 7.5 Transient loads The same principle as for permanent loads should be used. Where it is possible for only part of a load to be applied to the actual structure, (e.g. pattern loading), it is generally preferable to model each patch as a separate loadcase and use combinations to create the patterns. 7.6 Internal loads In addition to applied loads, other effects can change the distribution of forces within the structure, without applying a net force. Many of these effects can be modelled directly but extra care needs to be taken because the behaviour of the structure under these effects is less easy to check by hand. Checking the direction of the applied effect can often only be done by looking at the results. It is recommended that these effects are always modelled in separate loadcases from applied loads and from each other, to make checking as simple as possible. Temperature Unless a structure is free to expand and contract, the effects of a change of temperature need to be considered. Even if there is no external restraint to expansion, differential temperatures and temperature gradients across a member can introduce stresses. Care needs to be taken when using a uniform temperature change because in a number of circumstances spurious locked in stresses

can be generated which can be an order of magnitude higher than the ‘genuine’ stresses caused by a restraint to thermal expansion. To avoid this, temperature change must be applied to all the elements which span directly or partially between restraints (only truly transverse elements directly orthogonal to the line joining restraints can be omitted). However if any rigid constraints (including elements modelled with rigid ends) are in parallel with beams subject to temperature change (eg a grillage with rigid elements over the column width) they cannot expand and so will lock in stresses (temperature movements/stresses will also be underestimated if part of the element is rigid). Also if steel and concrete elements are in parallel (eg concrete slab members in parallel with primary steel beams) then if they have different coefficients of expansion, this will lock in stresses (which may or may not be considered spurious). Lack of fit If components are not exactly the right length then forces can be generated in those components and adjacent ones. This cannot usually be quantified at the design stage, and is deemed to be covered by partial factors, but may need to be considered if there is a problem on site. Prestress Prestressing will shorten the members to which it is applied, with similar effects to lack of fit and if the prestress is eccentric it will also introduce bending to the members. Unless the prestressed member is simply supported these distortions will introduce secondary stresses into the structure, which need to be considered, usually by applying equivalent loads to the model (section 11.17) 23/44

April 03


Support settlement Support settlement is another special case of lack of fit (section 8.4). 8 MODELLING RESTRAINTS General All structures are restrained to prevent global movement. If the whole structure is modelled then the model will normally be restrained where it touches the ground and the only decisions needed are on the rigidity of the ground. If only part of the structure is modelled however (e.g. a two dimensional frame which is stabilised by other structure out of plane), additional restraints (section 8.3) to the model are needed. Restraint at ground It is normal practice to assume initially that the ground is rigid and to allow for the effects of support settlement separately (section 8.4). Modelling the joint between the structure and the ground has the same problems as for other joints (section 3.3), but BS5950 states that if full fixity to the support is assumed, then a rotational spring to model flexibility of the ground should be used. A simpler approach is to analyse the model twice, once assuming pinned supports and once assuming full fixity and to use the moment from the fixed analysis for the design of the base connection only. Full fixity should only be assumed if both the connection and the foundation can resist the moments generated at the support without significant rotation (less than 10% of the rotation of a pinned member at that location). The use of rigid supports can produce very different reactions in adjacent supports which would in practice be evened out by very slight movements. If examination of the reactions shows this effect, a reanalysis using stiff springs (deflecting say 1mm under maximum reaction) is recommended. The sensitivity of the analysis to variations in this stiffness should be investigated. Raft Foundations Where a large building is supported on a ground slab acting as a raft, the stiffness of the soil, the stiffness of the raft and the stiffness of the structure above interact. Soil is not an elastic material and so using springs to represent it can be misleading. An iterative use of a soil displacement program and a structural analysis program where the spring stiffnesses are adjusted to match the predicted ground movements is recommended. A check should be made to ensure that any springs which end up in tension are deleted. Global restraints In a general 3 dimensional structure any point has six degrees of freedom, i.e. it can move in 3 directions and rotate about 3 axes. To simplify models it is possible to specify that every point is restrained in some of these directions. Such global restraints are selected automatically for some structure types (plane frames and grillages) where the plane of the structure is defined, but have to be specified by the user for other types (plane stress etc) where the structure can be in any plane selected by the user. Support settlement Differential settlement between supports can significantly affect the forces in a structure. When this is the result of different foundation conditions in different places it is not directly related to the magnitude of load and so cannot be modelled by a spring. Generally a maximum magnitude of differential settlement which might happen is defined and this has to be applied to each support in turn, using separate loadcases. 24/44

April 03


9 MODELLING FOR DYNAMIC ANALYSIS The mass of the structure and its contents is fundamental to its dynamic behaviour. Traditionally this has been modelled by specifying 'lumped masses' at nodes and assuming the model has zero density. It is now possible in some analysis programs to use the areas of the elements to determine the self mass, (which has the same disadvantages as using gravity to model self weight section 7.3) and/or to specify that a particular loadcase should be converted to represent mass. Because of uncertainties in material and element properties, there is not usually an advantage in using distributed instead of lumped mass in the analysis and whichever of the options given above is easiest to input can be used. The stiffness (section 6.2) of the structure is also fundamental to its dynamic behaviour. Non structural members like partition walls can significantly affect the stiffness of a structure under low amplitude dynamic loading. Further details are given in 'An Arup Introduction to Structural Dynamics' by Mike Willford. 10 INTERPRETATION OF RESULTS 10.1 Beams and columns Results from the analysis of the model of a skeletal structure (moment, shear and axial load) can often be used directly in member design. Exceptions include members where deflection affects the forces (section 11.3). Connection design needs to be considered carefully. In steel structures the capacity of the connection can often govern the design. To provide a connection capable of transferring the full moment capacity of the member might be impossible without haunching beams or stiffening tubes local to the connection. Except in the special case of portal frames designed plastically (where it is important that plastic hinges are formed away from the connection) the saving in weight achieved by minimising the member size is likely to be outweighed by the extra cost of complex joints. Stresses derived automatically for beams and columns can give a quick indication of whether members are grossly oversized or undersized but effects such as buckling mean that they are unlikely to be used directly for final design. 10.2 Slabs and walls Results from analysis of a slab or wall, either as a grillage of 1D elements (section 11.6) or a mesh of 2D elements, will generally need to be processed to derive values to use in design. Stresses in 2D elements which are modelling a uniform material like steel, can be used directly, provided buckling is not an issue. Stresses and derived forces in 2D elements modelling reinforced concrete need extensive post processing to derive design forces.(section 11.2) 11 ADDITIONAL INFORMATION

These topics are referred to in the main manual

25/44

April 03


11.1 Warnings and errors during analysis The three most common problems associated with a stiffness analysis are singularity, instability and ill-conditioning. The first two problems are easily spotted and can be easily rectified; the third is more difficult to spot, may sometimes be missed completely and is more difficult to cure. Where they occur, the model idealisation must be checked and the input data amended accordingly. Singularity Singularity occurs when the assembled structural stiffness matrix includes a diagonal term equal to zero. No solution can be obtained from such a matrix. This is normally due to lack of stiffness at a joint in a given direction or rotation. In practical terms, this generally does not imply that the structure is a mechanism but it does mean that some extra restraints must be applied so that the structure may be solved. Where torsion is likely to occur in the structure, a torsion constant of some value (even if it is very small) should be entered to prevent singularity. Global Instability Global instability differs from singularity in that all the nodes in the structure have a non-zero diagonal stiffness term but the structure is not restrained in one or more of its global degrees of freedom. Ill-conditioning Ill-conditioning is a numerical problem that arises during the solution of the stiffness equations, as a result of very large ratios between terms of the stiffness matrix. The problem is shown up in practice by the total applied loads at a node (including the fixed-end components from elements loads) not being equal to the sum of the element end forces of elements incident at that node. This is immediately apparent at the support nodes. Here the sum of the reactions in the global degrees of freedom not being equal to the sum of the applied loads in the corresponding direction is a sure indication of ill-conditioning. For non-support nodes, the problem is much more difficult to spot, unless the analysis program itself performs the "out-of-balance" check and warns the user appropriately. Large differences in the stiffnesses of elements meeting at a node are generally the cause of illconditioned structures; halving the length of an element by inserting an extra node may provide a solution. Another general rule is to avoid using relatively very large or small element areas and inertias, and to either fix or release the nodes attached to the elements instead. Zero areas and inertias will not cause ill-conditioning but may cause singularity. Referred to from section 2.5 Computer Analysis 11.2 Concrete Post processing of 2D element results Because concrete is usually designed as a cracked reinforced section, the stresses calculated from an elastic analysis of 2D elements cannot be used directly for design. Principal stresses are unlikely to be parallel to the direction of reinforcement. A method of converting in plane stresses into areas of reinforcement is described in Structures Note 1989NST_7 and use of a post processor for analysis data which automates this process and can allow for bending stresses as well is recommended. 26/44

April 03


Use of out of plane shear stresses to derive shear reinforcement is not recommended. These stresses can be used qualitatively to identify concentrations of shear force but punching shear checks should be done by hand at successive shear perimeters as described in the standards. Referred to from sections 3.4 – Slabs and 10 - Results.

11.3 P-delta effects

Normal static analysis calculations assume that displacements do not effect the forces in a structure. If a member carries predominately axial loads then deflection of this member will introduce second order, or P-delta, effects. For example, in a sway structure, the vertical loads generate moments. Design codes generally give rules for the design of elements to take account of these effects, such as by applying notional horizontal loads. In special cases, or where stipulated by the design codes, a full P-delta analysis to calculate these second order effects directly is required. There are no general rules for when a P-delta analysis should be carried out. A P-delta analysis should be considered if: • deflections are large resulting in P-delta moments greater than 10% of the static moment • a structure can sway, and no other methods of allowing for sway have been considered • compressive loads are high, so that buckling involving more than one member might be a problem If in this last case a P-delta analysis shows significant differences from a static analysis, a buckling analysis should also be undertaken to identify the critical buckling load directly. In a P-delta analysis there is a geometric, or differential, stiffness in addition to the normal structural stiffness. The geometric stiffness is derived from the forces in the structure, so the solution requires two passes. The first pass establishes the forces in the structure allowing the geometric stiffness to be established for the second pass. In a linear static analysis, provided the model is properly restrained, the structure should always be stable, so a solution is always possible. In a P-delta analysis this is not necessarily the case. If the axial force in an element is too high the elements may be unstable so that a solution cannot be found. Note too that since this is no longer a linear analysis, results from different load cases cannot be superposed.

27/44

April 03


P-delta analyses can be used to avoid using effective lengths derived from code rules, which do not apply directly to complex structural arrangements. Provided initial imperfections are included in the model, stresses from the analysis can be used to check an element directly; taking the effective length as equal to the element length. If a buckling analysis can be undertaken, the initial imperfections can be determined from the buckled shapes. Normally the deflection of the mode with the lowest critical load is scaled to an appropriate amplitude. This may be derived from the initial imperfection ratios used for appropriate elements in the code (see 1996NST_12 for advice to British and European codes) or be based on construction tolerances. Note that the initial imperfections make allowance for internal stresses as well as lack of straightness. Referred to from section 2.5 – Computer Analysis, 3.2 – Beams and Columns, and 10 - Results 11.4 Modelling castellated beams, trusses etc by shear beams The shear stiffness of a castellated beam, or of a truss modelled by a single beam element, is significantly less than for the equivalent solid beam and so shear deformations always need to be allowed for, even with slender beams. Suppliers of castellated and perforated beams supply proprietary software or design charts to use for their beams. The user needs to be satisfied before using such products that they are suitable for the particular application.

An accurate estimate of shear stiffnesses can be calculated by modelling top and bottom flanges and web members as beam elements in a plane frame. For scheme design the following rules should give an adequate approximation. In these formulae E is the Young’s Modulus and G is the shear modulus, and for an isotropic material with Poisson’s ratio ν:

E / G = 2(1 + υ )

Beam Type Castellated Beams It=I for T section at hole s = pitch of holes Vierendeel girders where elements are slender (element span/depth > 10) A = pitch of bracing members b = depth between flanges If = I for flange member Ib = I for bracing member Vierendeel girders where elements are stocky (element span/depth < 10) Af = area of flange Kf = shear factor for flange Ab = area for bracing member Kb = shear factor for bracing member

Bending stiffness (Isolid + I at hole)/2

Shear area E / G × 192 × It s2

E /G (I for top and bottom flanges)

(I for top and bottom flanges)

28/44

a a×b + 24 × If 12 × Ib 2

E /G a a×b E /G E /G + + + 24 × If 12 × Ib 2 × Af × Kf 2 × Ab × Kb 2

April 03


N-truss (pin jointed) E G × cosθ θ = angle of diagonal to horizontal (I for top and bottom 1 sin θ flanges) Ad = area of diagonal + 2 Ad × sin θ Av Av = area of vertical Warren Truss (pin jointed) E G × 2 × sin 2 θ × cosθ θ = angle of diagonal to horizontal (I for top and 1 1 Adc = area of compression diagonal bottom flanges) + Adc Adt Adt = area of tension diagonal

Referred to from section 3.2 - Beams and Columns

29/44

April 03


11.5 Modelling beams with long slots

Shear deflections in a member with a long slot will dominate. Two possible models are suggested. The solid sections are modelled in the normal way. The ends of these sections are then rigidly linked to nodes at the centroids of the sections above and below the slots and the slotted section is modelled by two elements.

The solid sections are modelled in the normal way. The slotted section is modelled as a beam with reduced shear area as follows: I for top and bottom sections about common centroid.

Bending stiffness:

E/G a a E /G E /G + + + 48 × It 48 × Ib 4 × At × Kt 4 × Ab × Kb

Shear area: where a = slot length A = area, I = inertia, K = shear factor for top (t) and bottom (b) sections

2

2

Referred to from section 3.2 – Beams and Columns 11.6 Grillage analogy for slabs A slab can be modelled by a grillage of 1D elements and this is generally appropriate where there are no in plane forces in the slab, or where the slab incorporates downstand beams. The longitudinal and transverse elements in the grillage should be given the axial and bending properties of the section of slab they represent. The torsional stiffness derived for the 1D element representing the slab (or the slab portion of an element representing a beam and part of the slab) must be halved, because both sets of elements contribute to the total torsional stiffness of the slab. (this sets the torsional stiffness GJ equal to the bending stiffness EI). Further guidance is given in CIRIA Report 110 and in 'Bridge Deck Behaviour' by E.C. Hambly (Spon, 1991). The results for a grillage consist of moments, shears and torsions. The bending moment diagram for a line of elements has a 'saw tooth' appearance because of the torsional moments in the perpendicular elements. This is a result of using discrete elements to represent the continuous slab but simply averaging the moments either side of a node will ignore the torsion stresses which is incorrect and unsafe. It is simplest and conservative, to add the average torsion per metre width in the four elements meeting at a point to the averaged moment. For more details on this and dealing with edge elements, see Structures Note 1991NST_16. Referred to from sections 3.4 – Slabs and Walls, 5 – Section Properties and 10 - Results

30/44

April 03


11.7 Setting up a model with 2D elements

Models using 2D elements have to be set up with great care if meaningful answers are to be obtained. The user must understand the fundamental difference between a 1D element and a 2D element. A 1D element is formulated to obey linear elastic beam theory, and so a single 1D element can be used to model a complete span, and will give answers which correspond exactly with beam theory. A 2D bending element on the other hand can be formulated in many different ways, and assumptions are made in these formulations about the relationship between out of plane displacements and rotations which mean that the results only approximate to those derived from plate bending theory. Different 2D elements can be used to model different effects. Elements in a 3D structure can model plane stress (in plane) and/or plate bending (out of plane) effects. Axisymmetric or plane strain elements can only be used in 2D models. 2D elements can have nodes at corners only (linear elements), or additional nodes along the sides (parabolic elements). Generally a parabolic element will give better answers for a given size of mesh, but linear elements can allow a finer mesh to be used without exceeding the capacity of the program. The ideal 2D element is a square, and the further the shape departs from this the less accurate the answers will be. The mesh of 2D elements in a model needs to be sufficiently small to ensure that the state of stress does not vary dramatically over the length of an element. For plate bending, typically eight elements would be needed to model a single span to give a sufficiently accurate model of the behaviour of a slab. For in plane stresses the mesh needs to be refined locally near stress concentrations to give acceptable answers, and a coarse mesh is likely to overestimate the stiffness of the element. Discontinuities of stress across element boundaries indicate that a plane stress model mesh needs refining. If less detailed models are to be used then simple test models which can be compared to hand calculations or a 1D element model should be analysed first to determine the likely accuracy to be obtained from the main model. Compatibility between 1D and 2D elements needs to be considered carefully when they are used in the same model. In particular if a 1D element is connected at one end to a node on the edge of a plane of 2D elements, and the 1D element lies in this plane, this is equivalent to pinning the 1D element to the 2D elements. Remember that 2D elements are only connected at nodes, and so trapezoidal elements need to be used for mesh refinement.

31/44

April 03


Referred to from section 3.4 - Slabs

11.8 Axis systems and element orientation

An axis system consists of three axes in orthogonal directions. These are usually righthanded axes systems:

Positive rotations about those axes follow the Right Hand Screw rule:

The fundamental axis system is the global Cartesian coordinate system. All other coordinate systems are defined relative to it. Each element is oriented relative to an axis system defined by its topology. Typically the default element x-axis runs from end 1 to end 2 of the element, and the default element zaxis is in a vertical plane. If a member is not orientated in this way in the structure the user must define its orientation in the model. Details of how to do this will be given in the program manual. x

Z Z

2

z'

z β

y

x 2

y'

z

y

1 Y

1

β

Y

X

X

Referred to from section 5 – Section Properties

32/44

April 03


11.9 Section properties for standard shapes To derive section properties from first principles the properties of standard shapes are needed. Such properties are given in textbooks and in documents like the Steel Designers Handbook, but some of the most common are given below: Section Solid Rectangle b > d

Area

b×d

Inertia

Torsion Constant

1 ×b×d 12

3

Solid Circle, π ×d2 π ×d4 4 64 diameter d Referred to in section 11.12 – Section properties

  d 4 4   3.36 × d  b  × 1 − b× d3 × 1 −  3 16 × b 12      or b × d 3 3 for thin rectangles

π ×d4

32

11.10 Multi storey frame models A number of tools have been developed to assist in the analysis of multi storey frame models, either by allowing simple ‘chassis’ models to be expanded to model a complete building, or to develop equivalent simple models during scheming or verification. Papers on these tools are held in R&D who can also suggest contact names for further information.

Referred to from section 3.4 – Slabs and Walls and 4.1 – Multistorey Buildings 11.11 Modelling bridge decks Bridge decks generally have clearly identifiable primary members spanning in one direction, supporting secondary members or a deck spanning in the other direction. Because bridges support moving concentrated loads, many loadcases are needed and so it is often beneficial to use comparatively crude skeletal models to model the slab decks. Influence lines can be used to identify worst locations for the application of load. If a distortion to an element in a skeletal model is applied, the deflected form of the model illustrates the influence line (or influence surface in 2D). Local effects of wheel loads on slabs are often calculated from influence charts rather than computer analysis. In this case loads on an analysis model should be applied to the primary structure to keep global and local effects separate. Details of methods of modelling different deck types are given in 'Bridge Deck Behaviour' by E.C. Hambly (Spon, 1991) and this book should be consulted for details. Referred to from section 4.6 – Bridge Decks

33/44

April 03


11.12 Section properties from first principles Second moment of area (Iyy, Izz) Complex cross sections can be divided up in to simple shapes. For each shape find the position of its own centroid, y, the area, A, and I for the shape about its own centroid (section 11.9).

∑ A× y ∑A

The position of the centroid of the whole section is then:

y=

The total second moment of the section is then:

Itot = ∑ I + ∑ A × y − y

(

)

2

Torsion Constant, (J) There is no equivalent set of rules for deriving torsion constants from first principles by adding components. Two examples illustrate this: • A tube with a longitudinal slot has a fraction of the torsion stiffness of an identical closed tube. • Open sections can be considered as a set of simpler shapes but the way a section is split into component parts can have a marked affect. The following questions need to be considered: • Is it a thin walled closed section? If so use the formula:

J=

4 × A2 ∑ (ds t )

• Is it a thin walled open section? If so treat it as a series of rectangles and use the formula:

(

J = ∑ 1 / 3 × ds × t 3

)

For thick walled sections more detailed guidance is given in Roark. Open sections should be split into rectangles, starting with the rectangle with the largest d * t ^3 that can be fitted within the complete section. For thick walled closed sections, where the hole dimensions are less than half the dimensions of the solid rectangle containing it, the hole can be ignored and the section treated as solid.

Referred to from section 5 – Section Properties 11.13 Modelling haunched beams The variation in stiffness along the length of a haunched or tapered beam can have a substantial effect on the distribution of forces and magnitude of deflections. It should be borne in mind that minor differences in stiffness due to haunching can have less effect than some of the other assumptions made during modelling (e.g. using gross uncracked section properties for concrete). Variations in depth of +/- 25% can generally be ignored. With greater variation in depth a haunched beam can be modelled by three elements, one representing each haunch, with I taken as the average of the support and span values (not the properties of an average depth section) and the middle one with the constant midspan section properties. Referred to from section 3.2 Beams and Columns

34/44

April 03


11.14 Modelling elements with rigid ends

Where members of substantially different stiffness are connected, for example where a coupling beam connects parts of a shear wall, an element connecting the centrelines of the shear walls will be too flexible. Assuming full fixity at the face of the shear wall would overestimate the stiffness, and so it is generally assumed that full fixity occurs at h/2 from the face, where h is the depth of the flexible member. Such a member can be modelled as a single element by increasing its stiffness. Determine the fraction N of the length which is flexible, then increase the stiffness by 1 3 N Alternatively the element can be modelled with rigid ends if the program allows this. Modelling the rigid sections by stiff elements is not recommended. Referred to from section 3.3 – Joints, and 3.4 – Slabs and Walls 11.15 Modelling beam and slab floors with in plane stresses The 'best' analytical model of the behaviour of a beam and slab floor under combined bending and in plane stress is a model where in plane forces are carried by plane stress elements and out of plane forces are carried by a grillage of elements with no in plane stiffness and reduced axial stiffness (modelling the part of the beam outside the slab depth only). However a model in this form produces answers which are very difficult to convert into reinforcement areas. For straightforward shapes a simple grillage (section 11.6), gives in plane deflections which only differ from the 'correct' answers by about 20%. In plane bending moments in the grillage elements generally cancel at nodes and can be ignored but axial forces need to be considered. If the slab is a complex shape or has many large holes in it then a plane stress analysis, neglecting in plane stiffness of the beams, (or the combined plane stress and grillage model described above) should be used to establish the behaviour of the slab under in plane loading. Unless this model identifies high in plane compressive stresses (greater than 0.2 fcu), or the depth of concrete in compression needed to resist bending in the beam elements exceeds 0.2d, it will be conservative to add the area of tensile reinforcement calculated from post processing the in plane stresses to the area of tensile reinforcement needed to resist bending in the beams. If these limits on compression are not satisfied then specialist help to determine reinforcement areas should be sought. Referred to from section 3.4.8 – Basement Floor Slabs

35/44

April 03


11.16 Symmetrical and anti-symmetrical models

Where only part of a symmetrical model can be included in an analysis because of limits on problem size which can be analysed by a particular program, only a half or a quarter of the structure needs to be modelled. Two different models, with different support conditions on the axes of symmetry need to be analysed, one used for symmetric loading and one for antisymmetric loading. Any load to be applied to the model can be split into symmetric and antisymmetric components. Support conditions for axes of symmetry in a plane frame are illustrated below: Symmetric loading

Anti-symmetric loading

Referred to from section 4.3 – Symmetrical Structures

36/44

April 03


11.17 Equivalent loads for prestressing

Prestressing a concrete beam imposes a set of loads on the beam which are in equilibrium. If the beam is simply supported it will distort under these forces without restraint but this distortion is prevented in continuous beams and secondary forces are generated. To determine the magnitude of these forces, a set of equivalent loads can be applied to the beam to model the effect of prestress. For the simplest case of a straight tendon in a constant section beam these forces will be applied at the ends of the tendon only. If the tendon follows a parabolic curve then in addition to the end forces a vertical uniformly distributed load is applied to the beam. If the position of the centroid of the beam section varies then additional forces are applied. The forces to be applied are summarised in the figure. Referred to from section 7.6 – Internal Loads

11.18 Properties of standard materials Basic ranges of properties for commonly used structural materials are given in the table below. These are based on data taken from relevant UK design standards and reference should be made to the relevant standards for prescribed values to be used when stiffness is critical. Material Steel Concrete (short term) Timber Wrought Iron Cast Iron Aluminium

Poisson's Ratio

Density

kN/mm² 200-210

0.3

kg/m³ 7850

Coefficient of thermal expansion strain / degree C 12e-6

20 + 0.2 fcu

0.2

2400

10e-6

N/A (4 - 7)

290 - 1080

0.25 0.25 0.3

7850 7850 2710

Young's Modulus

4 - 20 // 0.2-1.3 # grain 150-220 60-100 70

12e-6 12e-6 23e-6

Notes 37/44

April 03


Concrete properties are modified by creep under sustained loading, reducing the Young's modulus by a factor of 2 to 3. Further details on concrete properties are given in BS8110 Part 2. Properties for concrete in other countries (eg Hong Kong) are different. Timber properties are defined in EN 338 1995 Table 1. Referred to from section 6 – Material Properties 11.19 Holes in concrete beams (previously SGN 4.6) INTRODUCTION This Note describes a simple method for local analysis and detailed design around holes within the webs of reinforced concrete beams and ribs. It should not be applied to holes in prestressed or deep r.c. beams. (The latter are treated in the CIRIA design guide1 on deep beams.) No attempt is made to distinguish between holes that are structurally insignificant, and those that require design consideration. The distinction is influenced by a variety of factors including the size and location of the hole relative to both the depth and the span of the beam. The designer's own experience is a more reliable guide than arbitrary limits on size, although it can be said that any hole of length greater than nominal link spacing or depth greater than one-quarter the beam depth will certainly need to be investigated. If doubt exists with smaller holes, they should be checked.

BASIS The presence of a rectangular hole is assumed to change the behaviour of the beam or rib such that it acts locally as a Vierendeel frame. (Obviously if there are multiple holes at close spacing or if the hole dimensions are large in relation to the beam depth or span, the behaviour of the beam will be altered more radically, and a rigorous overall analysis may then be needed before local effects are considered.)

Holes of non-rectangular profile may be very conservatively simulated as a rectangular hole enclosing the extreme limits of the actual profile. But where the hole is of a shape that allows the beam to be simulated locally as a single or double lattice truss, having top and bottom booms and 'diagonals' which can be reinforced to carry loads across the hole, then it is both more realistic modelling and almost certainly more economical on reinforcement to adopt this truss analogy. Such an approach can be used when the hole is triangular, circular, or of a shape that can be inscribed 38/44

April 03


within an equivalent circle, but it should be limited to cases where the truss members framing the hole can be sized to have coincident centre-lines at 'joints' (thereby avoiding the need for a detailed analysis of local bending and force transfer at the joint). It must also be possible for diagonal bars trimming the hole to be bent alongside and lapped with the top and bottom reinforcement.

In practice these considerations will restrict the use of the truss analogy method to circular holes whose diameter is at most no more than one-third, and triangular holes whose height or length is no more than two-thirds, of the overall beam depth. Even these limits may be too generous for holes in shallow beams or those near the top or bottom of the beam. The term 'truss' is used to describe the analogy for modelling force transfer across the hole and, in practice, the analysis may well - for simplicity of working - assume that members are skeletal and pin-jointed. While this will give a 'safe' estimate of the axial forces to be designed for, it must be remembered that they are, in reality, squat members with monolithic joints, and detailing must take account of this. Forces are assumed to be transmitted across the hole as follows: Overall bending of the beam - by equal compression and tension forces having a lever arm which is the distance between the centroid of the concrete section in compression and the main tensile steel centroid

39/44

April 03


Vertical shear - rectangular hole, Vierendeel frame analogy: by shear and local bending across the hole. The distribution of shear between the concrete boom sections is dependent on the relative stiffnesses of the sections and on the effective span of these between notional points of fixity, which should be at least one-half the overall depth of the boom beyond the extreme end of the hole.

An applied vertical shear acting on a beam is carried across a rectangular hole by local shearing and bending of the boom sections. The distribution of shear between the booms can be determined from the assumption that the deflections of the booms across a hole are equal. An initial distribution can thus be made in proportion to the relative I values of the cross concrete sections (assumed uncracked): this will give a safe estimate of shear in the tension boom - which will probably be cracked - but may underestimate that in the largely or wholly uncracked compression boom. This can, conservatively, be designed to carry 100% of the shear; if that leads to unacceptably high stresses, the boom I values should be re-calculated allowing for long-term tension stiffening in concrete (as recommended in CP110) and an estimated percentage of tension steel. The design shear on the tension boom should, however, not be reduced from its initially estimated value; the total shear designed for in the two booms will thus exceed the actual value, but this is a

40/44

April 03


conservative approach to a difficult analysis which - if it underestimated shears drastically - could have equally drastic consequences. Vertical shear - triangular or circular hole, truss analogy: by components of compression and tension in the actual or notional diagonal sections adjacent to the hole and by shear across the joints where these intersect. The boom section spanning between the further ends of the diagonals may be assumed to carry only a nominal shear;

Local bending (due to loading applied to a boom section above or below the hole) - by bending of the section assuming beam action between fixity points (Vierendeel frame) or joints (truss analogy) adopted when assessing vertical shear transmission. Note that such loads can result in local tensions at boom ends which require extra tension steel to prevent tearing-out; Axial force (if present) - by axial forces across the reduced concrete boom sections. The applied axial force can usually be taken to act at the centroid of the gross concrete beam cross-section and can be shared between the top and bottom boom sections by simple statics (analogous to the sharing of load effects from a concentrated load on a simply supported beam, with the 'support' locations taken as the centroids of the gross concrete boom sections.

41/44

April 03


Note, however, that the local behaviour of a beam subject to a large axial force is similar to that of a deep beam on its side and a detailed investigation of the stresses and strains - e.g. by finite element analysis - may, in this case, be essential (but this is outside the scope of this Note); Torsion (if present) - by shear forces of opposite sign acting as a couple having a lever arm which is the distance between the centroids of the concrete boom sections, and by local lateral bending of these sections. Points of fixity are assumed at a distance beyond the extreme end face of the hole equal to one-half of the respective section width: a point of contraflexure will occur at the midspan of the section.

With a flanged beam, it is necessary to assess what flange width is to be considered as effective when defining the boom section. If the flange is in tension, it seems reasonable to take only the web or rib width into account. The same width should be assumed when considering vertical shear where the flange is in compression, while a greater width (suggested as the web width plus at least twice the slab depth) should be taken when bending, axial force, and torsion are being considered. 42/44

April 03


METHOD The method can be divided into four stages. 1. Establish the analysis model at the hole - Decide whether the hole is to be analyzed as an actual or equivalent rectangle by Vierendeel frame model, or as a triangle or circle using truss analogy - Sketch (to scale preferably) the actual or equivalent hole shape, and locate the centre-lines of the top and bottom boom sections (at the centroids of the gross concrete section), and of actual or notional diagonal sections if present (choosing a realistic breadth of section, related to the forces to be carried and the probable size of reinforcement cage to be used) 2. Establish externally-applied forces on beam and calculate corresponding local forces acting around hole - Determine the components of local forces due to each external force in turn, as described above 3. Check and design sections to resist local forces acting around hole - Assemble envelope of local forces on sections due to 'worst case' combination(s) of external forces - Check that sections can resist the individual and combined local forces including axial tension/compression, bending, and shear - Carry out detailed section design - Check section sizes adequate, allowing for cover, bars, space for concreting, etc. - IF SECTION INADEQUATE THEN EITHER REDUCE HOLE SIZE, INCREASE SECTION DIMENSIONS, OR ANALYZE MORE RIGOROUSLY 4. Prepare detailing instructions General - Check that detailed design satisfies durability and fire resistance needs (e.g. cover and fabric reinforcement) - Comply with relevant Detailing Manual2 recommendations for the beam or rib generally Main Steel - Check that all 'opening' re-entrant corners are reinforced with suitably anchored main bars along both faces - Provide crack control bars along all faces of the hole Links - Provide designed links where called for in booms (nominal links otherwise)

43/44

April 03


- Provide hanger bars (e.g. additional vertical links) to resist tensions due to local loading on the boom sections and shear at boom ends - Comply with recommended maximum spacing of links both laterally and longitudinally in relation to effective depth of reduced sections and diameter of longitudinal bars in compression Bends, Anchorages, and Laps - Ensure that longitudinal bars have adequate tension/compression anchorage beyond points of assumed fixity, and that diagonal bars are adequately lapped with longitudinal bars - sketch if necessary to ensure there is sufficient room - Specify 'slow' bends if needed for diagonal bars Buildability - Finally ensure e.g. by sketching that the details allow enough space for concrete to be placed. Referred to from section 3.2. Beams and Columns 12 REVISION HISTORY Revision A

April 2003

Section 3.2 refers to new section 11.19 instead of SGN 4.6 Section 3.3 new sentence on rigid constraints and dilation of 2D elements Section 7.6 new sentences on possible problems with temperature and rigid links Section 11.7 new paragraph on 1D to 2D connection Section 11.19 new section incorporating SGN 4.6

44/44

April 03

StructuralModellingManual_Arup.pdf

Recommend Documents