Solution Type

 

▒ Construction Stage Analysis

Construction stage analysis can be used to simulate the construction process of the ground using numerical analysis. Construction stage analysis consists of multiple stages and loading/ boundary conditions, as well as elements, can be added or removed at each stage. This loading/ boundary or element change is applied at the start of each stage. FEA NX can use following types of analysis features to conduct Construction stage analysis.

Stress-Slope Analysis

Analysis of stress and slope stability during the construction process

 

Seepage Analysis

Stage by stage Steady state seepage analysis, Stage by stage Transient seepage analysis

 

Stress-Seepage-Slope coupled analysis

Sequential Seepage-stress analysis and Slope stability analysis during the construction process

 

Consolidation analysis

Consolidation analysis for environment change and construction process of embankment

 

Fully-coupled Stress-Seepage analysis

Stress analysis fully coupled with Transient seepage phenomenon

 

Stress - Nonlinear Time History analysis

Users can perform nonlinear dynamic analysis considering stress status of ground resulted from not only self weight but also construction stage (the history of stress).

Nonlinear time history stage must be set at the final stage.

 

Heat Transfer

Stage by stage of steady state thermal analysis, stage by stage of  transient thermal analysis.

 

Seepage-Thermal Stress

Users can perform thermo-hydro-mechanical analysis.

 

Thermal Stress

 

Thermo-mechanical simulation can be conducted.

 

When conducting Construction stage analysis, the following should be considered.

  • Addition/Removal of element

  • Loading/Unloading of weight

  • Change in boundary condition

  • Change in rock material property

  • Definition of load distribution factor

  • Step by step underground water level

  • Drained-Undrained analysis

  • Initialization of displacement

  • Stress Analysis for initial construction stage (Consider Ko condition)

  • Restart

 

For example, the construction stages for a tunnel are as follows.

1 Stage: Initial ground stress

2 Stage: 1st face excavation

3 Stage: 1st reinforcement + 2nd face excavation

4 Stage: 2nd reinforcement + 3rd face excavation

5 Stage: 3rd reinforcement + 4th face excavation

…… (Repeat) ……

 

The first stage is the used to calculate the in-situ stress of soil strata. Because stress analysis of the ground assumes the in-situ state to be the initial state, the in-situ stress state needs to be calculated.

FEA NX uses self-weight analysis to calculate the initial in-situ stress.

 

Activate / Deactivate element

An element activated during Construction stage analysis has a default in-situ stress value of ‘0 (zero)’. But if a prestress is defined on the element, the element has the defined prestress value as its in-situ stress. If the self-weight is defined, the activated element has a body force due to its self-load. If the activated element uses the Modified Cam-Clay material model, it has an initial linear-elastic property that is determined by the loading/ boundary conditions of the corresponding stage.

New nodes will be activated as the element appears, and the initial displacement of the node is also ‘0 (zero)’.

If an element is deactivated at a construction stage, and an additional load distribution factor is not defined, the internal forces of the deactivated element are no longer considered. The total stress state is re-distributed according to this condition.

 

Loading / Unloading of weight

The addition and removal of load at each construction stage is possible and the load from the previous stage is maintained, except for following cases.

  • When an element subjected to the load is deactivated at a stage, its self-weight and external load applied to it are also removed.

  • When a node subjected to the load is deactivated, the external load applied to it is also removed.

Added load is cumulated to the already applied load from the previous construction stage.

Boundary conditions can also be modified in the same way and the same exceptions hold true.

 

Load distribution factor

The Load distribution factor is used during Construction stage analysis to simplify the modeling. The Load distribution factor is a numerical analysis method that uses the load distribution factor to apply the effects of element removal sequentially in the following stages. The Load distribution factor can be used to simplify a 3D problem in 2D, or to downscale the construction stage of a 3D model during analysis.

For example, if stress relaxations of 40%, 30% and 40% are assumed to occur in three consecutive stages, starting from the excavation stage, define the excavation stage and activate the load distribution factor option for that step. Input 0.4, 0.3 and 0.3 for the load distribution factor in option window for ‘After Current Stage 0, 1, 2 stage’ respectively.

 

Material property conversion

During Construction step analysis, the ground material properties can change to model time dependent ground disturbance, soil improvement or hardening. There are also cases where the structural material properties need to be change in the middle of the stage, such as hardening of lining concrete or changes in lining thickness. For this purpose, the material properties of a specific element can be changed without any number limits. The changed material property is continued onto the element results(displacement, stress, strain etc.) of the previous stage for analysis.

Caution: The Material property conversion feature needs to be used carefully. Changing the infill material after excavation in Construction stage analysis can be simulated using just the property conversions, without activating or deactivating any elements. Here, the stress conditions from the previous stage is applied to the following stage and so, physically inappropriate behavior can be observed due to the material property conversion. Hence, the material property conversion needs to be conducted at a stage where the element is deactivated and re-activated to obtain the intended results. If a new element is activated, the internal element has an in-situ stress, strain and interior state variable of ‘0(zero)’.

 

Undrained Analysis

Undrained analysis can be conducted for selected elements and selected construction stages. Two conditions should be satisfied beforehand to apply undrained analysis. Firstly, the drainage parameter should be set as undrained type on material model. Secondly, the undrained condition should be checked on the Analysis control of construction stage. If only one of the conditions is met, the material conducts drainage analysis in the corresponding stage.

For singular analysis cases such as static linear/nonlinear analysis, or slope stability examination, check the Analysis Control > Undrained Condition > Allow Undrained Material Behavior.