[STRAUS Applications] [STRAUS Specifications]
[STRAUS Users Page] [STRAUS Model Archive] [Technical Papers and Tips Contents Page]
[Technical Articles Contents Page] [Home Page] [Previous Page]

Using STRAUS to analyse steel structures to AS 4100

Dr Paul Cain, BE PhD RPEQ
Consulting Structural Engineer

This article refers to structures modelled using beam elements to represent beams and columns, that are to be analysed with an elastic analysis in accordance with Clause 4.4 of AS4100. STRAUS is able to perform all the analyses called up in this Clause viz a first-order elastic analysis (the linear static solver), a second-order elastic analysis in accordance with Appendix E (the nonlinear static solver), and an elastic buckling analysis in accordance with Clause 4.7.2 (the linear buckling solver).

Firstly I would like to try and put Clause 4.4 in perspective. I suggest that it is sufficiently accurate to design most members, including sway members, to the lower tiers of AS4100, using a linear analysis without any moment amplification at all. This is comparable to design to AS3990 (Ex AS1250). My experience and the feedback I have had from others is that the amplified moments obtained from a nonlinear analysis are generally not significantly larger, so that members generally do not increase in size. This does require engineering judgement as to when critical load combinations should be checked with a nonlinear analysis. Very significantly, it means that Clause 4.4.2 can be crossed out!

First-order elastic analysis
Clause 4.4.2.1

A linear analysis is the simplest and quickest of all options. However Clause 4.4.2.1 requires the moments obtained to be increased by the use of moment amplification factors (b or (s calculated in accordance with Clause 4.4.2.2 or 4.4.2.3 In general, these will vary for each member and for each load case or combination. These are relatively difficult to calculate by hand, and it would be unrealistic to attempt to do so except for small models with only a limited number of load cases. It is possible to calculate (s by hand methods for some simple structures. For more complex ones, it is necessary to use a linear buckling analysis to calculate the elastic buckling load factor (c as described below. It would be possible for a steel design module to evaluate (b relatively simply but not (s Having calculated (b and (s Clause 4.4.2.1 requires a nonlinear analysis if they are greater than 1.4. In practice such large values are uncommon even for sway frames like portals whose design is likely to be governed by deflection. The magnitudes of (b and (s are generally so small that it is much simpler to ignore any moment amplification and be a little generous in sizing the members; eg. by using a lower tier interaction formula for combined bending and axial loads as per Ref (1). This particular formula is so much simpler than those in AS4100 that it is a win win situation for hand calculations. It is relatively simple to confirm this by doing a nonlinear analysis of the critical load combinations.

Linear buckling analysis to
Clause 4.7.2

Clauses 4.4.2.3 (a) (iii) and 4.4.2.3 (b) require a separate linear buckling analysis in accordance with Clause 4.7.2 for each load combination. The STRAUS linear buckling solver can be used but the current version will only do 1 load case at a time, and will not do load combinations. It is therefore necessary to combine all loads into individual stand-alone load cases. If more than one load case is required, multiple runs of the buckling solver are required. These could be executed on the same model for each load case or alternatively the model and results could be saved under another name and the buckling runs could be performed on each new model. The elastic buckling load factor (c is the lowest positive eigenvalue. I suggest that the first 4 eigenvalues be calculated, in case some are negative. Negative eigenvalues have no real meaning (unless the forces can change sign), so simply ignore them. The buckling solver requires a linear static run first. It has the advantage of being a lot quicker to solve than a nonlinear analysis; about 2 minutes compared with 15 minutes for the portal described below. However I think buckling analyses should be restricted to simple models only, such as 2 dimensional portal frames, and even then I think a nonlinear analysis would be simpler and quicker overall. The difficulty with buckling is in ensuring that the buckling mode corresponds to the bending mode for that particular load case. This means that all restraints must be accurately modelled, which is not as simple as it sounds. Consider for example the simple 2 dimensional portal frame shown below which is loaded in only 1 plane. It does not require out of plane restraints to be included for a linear analysis. However the restraints must be fully and carefully modelled in order to prevent out of plane buckling for a buckling analysis. For a large 3 dimensional model with a number of load combinations, this could easily become a nightmare. I think it much simpler to use the nonlinear solver which uses the same model as for the linear analysis.

Second-order elastic analysis

This can be done using the nonlinear static solver, and selecting the Include [Kg] and Geometric Nonlinearity options, but not the Material Nonlinearity option. The No. of Increments should be set to 1. (There is no need to set more than 1 increment unless the structure undergoes very large deflections. For typical engineering beam structures, the overall deformation should be sufficiently small to ensure convergence is achieved without the need to progressively apply the load.)

The model is the same for both linear and nonlinear solvers but the nonlinear solution is an iterative one which takes much longer than a linear analysis. For this reason it is best to debug the model using the linear solver and ensure member sizes are correct before running the nonlinear solver.

A significant difference between the linear and nonlinear analyses is in their treatment of load combinations. In a linear analysis, the results of individual load cases are combined after the analysis. In a nonlinear analysis the loads must be combined before analysis.

The load case or combination of load cases to be analysed is specified by selecting Load in the Nonlinear Solver Panel. This is completely separate from Combine Results Files which is accessed from the main menu for linear static runs. Only one load case or combination can be solved at a time. If more than one load case or combination is required, the model and results must be saved under another name. (Use Back-Up Structure on the main menu and select All Data). Unlike the linear solver, it is necessary to subdivide each member into a number of elements to improve the accuracy. This also increases the speed by improving convergence. For most engineering structures which involve relatively small displacements, 3 such elements should be adequate.

This is clearly illustrated by the results tabulated above for a simple portal frame model used as a benchmark by Hancock (2). The numbers in the second column of the table, refer to the number of elements into which AB,BC,CD are each subdivided.

Note that increasing the number of elements reduced the number of iterations required and reduced the solution time. Also, the linear analysis gives a large error in displacement but a relatively small error in bending moment.

References:

1. Steel Structures Design Handbook published by Standards Australia.
   
2. Second Order Elastic Analyses Solution Techniques And Verification by G.J. Hancock published in Steel Construction, Vol 28, Number 3, Sept 1994.
   

For more information please contact us by e-mail: hsh@iperv.it