Analysis

Contents

• Improvements and speed up of analysis calculations
• Improved construction stages
  • Time-dependent analysis
    • Procedure steps and settings
    • Calculation procedure
    • Compatibility with the simplified modeling
    • Limitations
  • Removal of temporary objects
• Minimum division number for edge connections

Improvements and speed up of analysis calculations

FEM-Design 22 comes with a significant increase in performance.

The performance acceleration is noticeable in all types of analysis calculations (including non-linear). This is achieved by parallelization and refactoring of matrix assembly and solver algorithms, as well as improvements in processing and application of finite element mesh.

Additionally, stability and dynamic calculations are accelerated thanks to the improvements to the existing eigen-solver (Subspace method) as well as introduction of a brand new eigen-solver - i.e. Krylov/Feast method, which is characterized with the following advantages:

• It finds only the positive critical load parameters.
• The Sturm-check is not needed.
• Restarts required when searching for mods that belong to 90% of the modal mass are faster.

Improved construction stages

FEM-Design 22 comes with two very significant enhancements to the construction stage-based analysis of load-bearing structures. These are:

• time-dependent analysis, and
• option to remove temporary objects.

Time-dependent analysis

In FEM-Design 22, time-dependent analysis (TDA) has been implemented in order to model constraint creep, concrete material shrinkage and elastic moduli increment during time. The main feature are as follows:

• Visco-elastic materials
• Capable to model time dependent creep, constraint creep and relaxation
• Capable to model time-dependent shrinkage
• Capable to model time-dependent elastic moduli
• Support of Eurocode for concrete structures
• Support of Eurocode defined non-linear creep final value
• Support of Creep compliance for concrete/steel/timber structures
• Support of Prony series for concrete/steel/timber structures
• Compatibility with the Eurocode-defined, simplified elasticity moduli changing method for Creep
• Support of real beam/column/truss, plate/wall, and profiled plate/wall structural elements
  
   

The following animation shows a simple example of change of deflection over time (according to construction stages):

Procedure steps and settings

Step 1

For any structural element in the TDA, TDA properties under its Default settings > Material > Application data shall be defined.

Creep models

There are 3 creep time dependent analysis models available in FEM-Design 22:
 

1. EN 1992-1-1:2004

It is only available for concrete structures and follows the EN 1992-1-1:2004 Annex B1 defined parameters. t₀ has special meaning, because it is also the age of the structural element when it is applied in the structure due to its construction stage.

Non-linear creep consideration
If this option is enabled, the software checks the compression internal normal forces and calculate the non-linear creep final value according to EN 1992-1-1:2004 3.1.4. (4). If the Allowed to increase final value during lifespan option is enabled, this examination will be executed in every time step and increase final value if it is necessary. Otherwise, only the activation moment of the structural element will be examined as the code-called first loading.

The linear creep final value is independent from the f_cm, but the non-linear creep is not if the age of concrete is under 28 days, consequently, Cement type information is needed. The non-linear creep consideration is disabled by default because it could cause performance downgrade.
 

2. Creep compliance by Data set

The normalized creep compliance could be defined by a time dependent data set for Concrete, Steel and Timber materials.
 

3. Creep compliance by Prony series

The Prony series is the classical general approach to model visco-elastic materials. Creep compliance could be approximated by Prony series using the following summation:

where j(t) is the creep compliance, ,   and  are compliance and retardation time of the ^th element of the Prony series respectively [1, 2].

Example: A Creep compliance data set could be approximated by a simple function fitting using least-square method [2, 3].

Major advantage of this approach is that the below-mentioned hereditary integral solution could be formulated without the convolution, and the kinematic increment in the t_i+1 time point could be calculated from the known, previous state t_i and the  time step thus, allowing to have less state variables. Hence computational and memory demand is lower than continuously evaluating the historical effects of the full time history for each step.

The major drawback is the numerical stability: not properly fitted curve or unfavorably chosen timestep (by Construction stages) could cause numerical artifacts, like oscillating results.

Many literature represents the General Maxwell rheology model in the following form and defines the corresponding Prony series for the relaxation modulus using the: elastic moduli; and   relaxation times [3, 4].

For the same model the creep compliance can be defined analogously to the relaxation modulus [4] and Prony series can be given using fitting processes [2, 3]. The software requires the approximation of the creep compliance. Because of this if only relaxation data is available for a specific material than conversion between relaxation modulus and creep compliance have to be applied [4, 5].

In case of a one element Maxwell model the conversion defined by the convolution integral of [4, 5] can be given simply as:

Shrinkage models

There are 2 shrinkage time dependent analysis models available in FEM-Design 22:

1. EN 1992-1-1:2004

Eurocode defined shrinkage effect is modeled, using the parameters according to chapter 3.1.4. (5) and Annex B2.

2. General

It can be defined in a table form, where the value of shrinkage is set by time. Below the user-defined time-value, the software assumes zero shrinkage, and above - the last shrinkage value.

 

Elasticity models

There are 2 elasticity time dependent analysis models available in FEM-Design 22:

1. EN 1992-1-1:2004

Eurocode method given by EN 1992-1-1:2004 3.1.3.(3) has been implemented.

2. General

General method allows to define unique elasticity modulus multiplier over time in table-based form. The user-defined function should be monotonically increasing.

Step 2

Setup the construction stages together with their end time (Time).

Step 3

Setup the active load cases by stages together with their multiplier by limit states (U, S_c, S_f and S_q). If there is no activated load in a construction stage, then only the time-independent changes will be felt and taken into account.
 

Step 4

In order to run the analysis according to the construction stages as time-dependent, one has to turn it on with a separate option.

The Creep strain increment limit controls the size of the kinematic load caused by creep. If the kinematic loads are bigger than the control allows, the actual time step will be reduced. High values are fit to determinate structures where the creep would not cause internal force redistribution. Low values are fit for highly constraint creep or relaxation phenomenon.

Calculation procedure

The calculation method uses a hereditary integral for creep modeling.

Where  is the creep compliance.

This equation could be reformulated into:

Where the first multiplication is clearly the elastic strain, and the integral part is clearly the creep strain [4].

The TDA calculation uses time steps, where in each timestep, the creep strain increment of the time step will be applied as a kinematic load, calculated from the elastic strains of the prior state.

In case of a determinate structure, no internal force redistribution will occur when the kinematic loads will be applied, so one timestep could be performed without any precision penalty. But an arbitrary, indeterminate structure could have major internal force redistribution, which will enforce to smaller timesteps. If the model’s internal forces would have not converged, the software automatically reduces the timestep, but it has much higher performance penalty than limiting the creep by the elastic strains before the analysis step.

Compatibility with the simplified modeling

The default creep modeling procedure in FEM-Design is the so-called simplified method, based on the modification of the elasticity modulus. This option is available for the Eurocode highlighted limit states: U, S_q, S_f, S_c.

During TDA calculation this modeling option is also available, which means that the elasticity modulus could be modified by the above-mentioned options, and these will be applied if the structural model does not have set time-dependent Creep model. 

If any structural model, or construction stage load setting have different settings by limit states, it will enforce multiple calculations, in the worst-case scenario, 4 TDA calculations. 

Limitations

• Shear strain is not considered in additional creep strain calculations.
• In the case of concrete materials, the visco-elastic behavior is considered on pure concrete cross-sections without cracks. (Cracking effect could be modelled with the stiffness modifiers if necessary.)
• In the case of fully unloaded structure, there is no remaining strain due to its nature of the visco-elastic behavior.
• Post-tensioned cables do not have time-dependent properties and any interaction with this feature, so during the TDA calculation, it will be handled as a usual load system.
• Shrinkage and elasticity increasement modeling is only available for Concrete material.
• During TDA calculation, shrinkage load will be applied with the value of the defined TDA model, if applied reinforcement exists, it is considered using uncracked cross-sectional properties.

[1] Haj‐Ali, Rami M., and Anastasia H. Muliana. "Numerical finite element formulation of the Schapery non‐linear viscoelastic material model." International Journal for Numerical Methods in Engineering 59.1 (2004): 25-45.

[2] Park, S. W., and Y. R. Kim. "Fitting Prony-series viscoelastic models with power-law presmoothing." Journal of materials in civil engineering 13.1 (2001): 26-32.

[3] Kraus, M. A., and M. Niederwald. "Generalized collocation method using Stiffness matrices in the context of the Theory of Linear viscoelasticity (GUSTL)." Technische Mechanik-European Journal of Engineering Mechanics 37.1 (2017): 82-106.

[4] Reddy, Junuthula Narasimha. An introduction to continuum mechanics. Cambridge university press, 2013.

[5] Sorvari, Joonas, and Matti Malinen. "Numerical interconversion between linear viscoelastic material functions with regularization." International Journal of Solids and Structures 44.3-4 (2007): 1291-1303.

Removal of temporary objects

Until FEM-Design 21, structural elements could only be added to the previous construction stage. From now on however, structural objects (as temporary elements) can be removed from the different construction stages, and most structural elements can even be removed from the later construction states to simulate temporary elements or other engineering problems.

The temporary elements (structural objects) that can be removed from the later construction stages:

• Bars: beams / columns / trusses / fictitious bars
• Connection elements: point-point, line-line and surface-surface connections
• Support elements: point, line and surface supports

Procedure

First, just as in version 21, one should define at least two different construction stages. After that, when the construction stage dialog is active, the temporary structural elements (structural element to be removed) need to be reassigned to those construction stages in which they are active.

Example 1:

There are 4 construction stages defined, and one of the structural objects should only be active in the first 2 of them. Following steps should be performed:

1. Open Construction stages dialog.
2. Select from the first combobox the starting stage of the structural object when it should be active (e.g.: first stage).
3. Select from the second combobox the last stage of the structural object when it still active (e.g.: second stage).
4. Select the relevant structural object from the model space.

Following these steps, the selected structural object will be reassigned to the first two stages and removed in the rest of them. To summarize, one shall simply assign the objects to the appropriate (from to) stages using the Construction stages command.

Example 2:

In the following example, a beam is extended with another beam, then a rotational support is added to the independent endpoint of the first beam, and finally the middle support is deleted.

The My bending moment diagram changes over time based on the assignment of the beams and supports to the stage.

Example 3:

The following animation shows an example  when a support column was removed from under the constructed top floor in the 3rd stage.

Minimum division number for edge connections

So far, it was possible to set a default minimum division number for bar objects. From now on, it is also possible to set a default minimum division number for edge connections. This is a time saving function in the modeling and calculation of prefab shells, where the “Separate end point from environment” behaviour is used (it requires at least three finite elements per edge).

Set the Default minimum division number for Edge connection under Setting > Calculation > Mesh > Elements.