It’s time to get back to the analysis of the stresses and strains in the dome of the Cathedral of Santa Maria del Fiore in Florence.
Since the last installment I have purchased “Brunelleschi’s Cupola” by Giovanni and Michele Fanelli, which is an excellent two part book covering in Part 1 the architecture and history of the structure, and in Part 2 an account of the engineering aspects of the structure, including a detailed account of finite element analysis studies carried out in recent years. This book provides an excellent source for the structural details of the cathedral, of which it has proved difficult to find reliable information elsewhere. The book is an english translation of an italian text, which makes it heavy going in places, but the plentiful and excellent illustrations more than make up for that. On the question of whether “cupola” is the right term for the world’s largest masonry dome, see Just What IS a Cupola Anyway?.
In the analysis which I will be reporting here, rather than just repeat the work already covered in the book, I will be building up a progressively more detailed model, starting with the dome alone, then adding the supporting structures, and finally investigating the effects of long term changes such as creep and the effect of seasonal temperature changes. All analyses were carried out using the program Strand7.
The model used for the first stage is almost the same as presented previously, the only difference being that a second material type has been introduced, so that the lower 6 metres can be modelled as stone construction, and the remainder as brickwork. Two analyses have been run with two different base support conditions:
- All base nodes fixed in all directions
- All base nodes fixed vertically, end face nodes fixed in the Z (circumfrential) direction, and one central node fixed in the X direction
In both cases the end face nodes were fixed in the Z direction over the full height to provide symmetry conditions. The two models represent the possible extremes of the restraint provided by the supporting structure in the radial direction; that is either fully fixed or no restraint. Later models will come closer to modelling the actual degree of restraint in the radial direction, and also include the effect of variable support in the vertical direction.
Each of the two basic models were analysed by two different procedures:
- Linear elastic with all loads applied to the complete model in one stage.
- Staged construction, with the model built up in layers, following a simplified model of the actual construction sequence. Linear elastic material properties were also used for this analysis.
The results of the single stage analyses are shown below. Since the purpose of the analyses is to reproduce the cracking pattern seen in the actual structure the results will concentrate on the circumferential stresses (stress TT), and only tensile stress contours are plotted:
To carry out a staged analysis the structure is divided into groups, which are then allocated to a sequence of construction stages, and finally load and freedom cases are allocated to each construction stage. In Strand7 it is possible to set up the stages automatically, but it is important to ensure that the various options are set correctly. With the default settings applied to this case the staged analysis (with linear material properties and linear geometry) gives exactly the same results as the single stage linear elastic analysis. The reason is that by default when each new group of elements is added to the model they are stretched and compressed to match the strains in the elements they are connected to. To model the construction of structures in masonry or concrete or similar materials the “morph” option must be selected, as shown below, so that the new elements are re-sized to match the deformed shape of the structure, without introducing additional stresses into the new elements.
See the Strand7 for details of the other morphing options.
Having set the morph option for all stages other than the first, the analysis gives significantly different results for both the fixed and free base options, as shown below:
It can be seen that with the alternative options for construction stages and base fixity the maximum stress ranges from 60 kPa to 1000 kPa on the inside face, and 150 kPa to 750 kPa on the outside face. In the next instalment we will look at the effect of including the supporting structure in the analysis to narrow down this stress range, and also to model significant effects not included in these preliminary analyses.