There are certain things that are unavoidable in life. Death, taxes and concrete cracking… right? Modelling cracked behaviour of concrete is an important step to ensure that your analysis is accurate and a true representation of the real life behaviour of your structure. This article explores how to model cracked shear wall behaviour in ETABS using stiffness modification factors.

**Cracking occurs in concrete when the tensile forces within the concrete member exceed the tensile capacity of the concrete due to a combination of tension, bending and shear forces. Although steel reinforcing is generally provided in concrete members to support tension forces, the process of concrete cracking can significantly reduce the stiffness of the member.**..

## The Mechanics of Cracking in Concrete Members

Before jumping into our FEA analysis software, lest touch on a very basic first principles concept.

Considering a very simple rectangular concrete member in bending, cracking does not occur at low levels of loading. This means that the section is un-cracked and therefore the full cross-sectional area is effective. This results in a simple bending stress distribution in the cross-section with tension in one half of the member and compression in the other half…

The stiffness of the member is effected by its Young’s modulus “E”, as well as its Second Moment of Area “I”. The second moment of area for a rectangular section is given by…

As the bending increases in the member, the stress will eventually reach a point where the tension capacity of the concrete is exceeded. At this point, the tension reinforcement provides the resistance to the tension within the section. The cross-sectional area of the tension reinforcement in the tension zone contributes to the stiffness of the member, the concrete within this zone no longer contributes to the stiffness of the member after cracking has occurred.

The stress distribution within the same section will now look like this…

The cracked zone in the concrete member is represented as the white space in the cross-section image above.

The reduction in effective cross-sectional area of concrete due to cracking is a phenomenon which needs to be accurately accounted for in your structural analysis . But why?…

## Why Modelling the Behaviour of Cracked Concrete Members is Important

There are two main reasons why modelling this behaviour in your analysis is important:

- The reduction in cross-sectional area of concrete reduces the members stiffness. If this effect is not accurately accounted for, the movement and deflections within your structural analysis will be lower than the real life behaviour of the structure. This may result in non-code compliant building movements.
- Accurate cracking assumptions is important for a structural system comprising multiple separate systems supporting the same load. An example of such a system is a building stability system comprising multiple cores and shear walls or a coupled core and outrigger system (to learn more about stability systems in buildings see THIS article). The proportion of loading which each element supports will be dependant on the level of cracking within those elements. The level of cracking effects the stiffness of the member and therefore how much load it “attracts” in a given system.

## Modelling Cracked Behaviour of Shear Walls in ETABS using Stiffness Modifiers

Now that we know the mechanics of cracking in concrete members and the importance of modelling this behaviour accurately, lets now take a look at how to mimic this behaviour for shear walls within ETABS.

The cracking behaviour of shear walls (or any other member for that matter) within ETABS is performed using factors called “Stiffness Modifiers”. This can be found my navigating to the following location…

**Assign >>> Shell >>> Stiffness Modifiers…**

The following dialog box then appears…

From this dialog box we can see that there are a number of stiffness modifier options to choose from. In order to use this dialog box effectively, you must first understand the axis convention that ETABS uses.

For this application ETABS uses a 1,2 and 3 axis system. Lets take a small portion of a shear wall modelled vertically in ETABS with its corresponding axis assumptions…

This diagram may look elaborate and complex, however if we break it down into elements, it becomes quite intuitive…

The coordinate system 1, 2 and 3 represents the left-right, up-down and in-out directions on screen (simple enough!).

Each face of the wall cube is then given a name. **The name of each face corresponds to the axis it runs perpendicular with**. For example…

- Face 1: Is the left and right faces (perpendicular to axis 1)
- Face 2: Is the top and bottom faces (perpendicular to axis 2)
- Face 3: Is the near and far faces (perpendicular to axis 3)

The axis convention for each stiffness modifier within ETABS is then given by a force (axial, shear, or bending or F, V and M respectively), followed by the name of the face, then followed by the direction of the force in question. Or in other words simplified like this…

So the stiffness modifier F22 corresponds with:

- An axial force
- Acting on face 2
- Acting in the up or down direction

## What Stiffness Modifiers Should I use for Shear Walls in ETABS

Now we can decide upon the Stiffness Modifiers we actually want to modify for a cracked shear wall.

As far as ETABS is concerned, shear walls, whether as a stand-alone wall or part of a group of walls say within a core for example resist bending along its major axis through a push/pull coupling of compression an tension forces.

This means that it is the “F” stiffness modifiers we are interested in modifying. Namely:

- F22 (vertical tension or compression)
- F21 (horizontal shear)

In addition to this, it is usually not the intent for a shear wall to support large magnitudes of loading through bending about its weak axis (i.e. out-of-plane bending). For this reason, Structural Engineers will often apply a nominally small stiffness value to the out of plane bending parameters, namely:

- M11 (bending about axis 1)
- M22 (bending about axis 2)
- M12 (twisting effect of the shell)

For modelling a header beam as a shell element (or coupling beam or lintel beam… the name differs depending on your region), you will then be interested in the “horizontal” stiffness modifiers for this element, namely:

- F11 (horizontal tension/compression which is regarded as in-plane bending behaviour of a shell element in ETABS)
- F12 (vertical shear of spanning header beam)

## Cracked Section Values as per ACI318

The American Concrete Design code ACI318 provides guidance on stiffness modifiers to adopt for varying structural elements depending if they are cracked or uncracked. There is a simplified table approach, or a calculated approach. Here is the simplified table which is a reproduction of ACI318…

Structural Element | Modifier (Ultimate) |

Columns | 0.70 |

Walls (Uncracked) | 0.70 |

Walls (Cracked) | 0.35 |

Beams | 0.35 |

Flat Plates and Flat Slabs | 0.25 |

ACI381 also gives allowance to increase these factors when assessing serviceability behaviour of a structure (deflection, drift etc.). These values are achieved simply through multiplying the values in the previous table for the ultimate condition by a factor of 1.43

Structural element | Modifier (Serviceability) |

Columns | 1.00 |

Walls (Uncracked) | 1.00 |

Walls (Cracked) | 0.50 |

Beams | 0.50 |

Flat Plates and Flat Slabs | 0.35 |

## Cracked Section Values as per AS3600-2018

The Australian Concrete Design code (AS3600) has guidance of is own on the modifiers to use for cracked and uncracked sections.

For uncracked sections, AS3600 simply allows the gross cross-sectional area (and therefore gross second moment of area) value to be used.

For cracked sections, table 6.2.4 is used. Here is a snippet below…

The AS3600 approach is slightly different to ACI318. I prefer the ACI approach as it is a quicker process to derive your cracking values if you are working within an FEA model such as ETABS.

## Practical Example for Modelling the Cracked Behaviour of Shear Walls in ETABS

Lets take a look at a really quick example to see this in action.

Our example shear wall has the following characteristics:

- 300mm thick (or 11.8 inch)
- Concrete grade of 80MPa (or 11,600 psi)

The first thing we need to know is what is the tensile stress of the wall when it cracks. This is found in your local Concrete Design Code (wherever you are located). For Australia, it is found in AS3600 3.1.1.3. Here is the equation…

f_{ct.sp} is the splitting tensile stress of the concrete itself. Here is the equation for that one (found in the same clause 3.1.1.3…

f’_{c} is the concrete grade (in our case 80MPa). Therefore our tensile capacity of the concrete (the point at which it will start to crack), is given by…

f_{ct} = 0.9 x 0.36 x 80^{0.5} = **2.90 MPa**

Now we are assuming you have a fully modelled structure in ETABS, which is correct and free from errors. For some great tips on how to ensure that your ETABS model is correct, take a look at THIS previous article.

Typically you would then run your analysis firstly assuming un uncracked section, then survey the stress results of your shear wall. For this example, we are looking at a serviceability wind case for this shear wall. The shear wall is part of a group of walls which make up a core for a multi-level office building. The cracking to the wall is quite extreme.

Lets take a look at the stresses in our wall. To look at these you need to navigate to the “Display Shell Stresses/Forces” toolbar button (or alternatively press F9). Here is what the toolbar button looks like if you are searching for it…

The following dialog box will then appear…

With reference to the numbers on the dialog box above, here is a quick explanation of each point:

- You can chose either case, combo or mode result. I am looking at an envelope load combination for this check so I am choosing combo, its really dependant on what load you are checking for for your specific shear wall.
- The name of the load or load combination you wish to view the force/stresses for.
- You can chose Absolute max, max or min for the stresses you would like to observe. Because we are interested in tension, we want to see the maximum results for the stresses (in ETABS positive values are tension, negative values are compression).
- You can either view stresses, forces or strains with this drop down box. Because we already know our cracking as a stress, for easy comparison we will be looking at the tension stresses within the wall.
- Again, we want to see the maximum stresses in the wall, this drop down box however allows you to view the stress for the visible face, top face, bottom face, max, min or absolute max.
- We are interested in the vertical load direction on the horizontal plane of the wall (or F22 if we are referring to the previously outlined axis convention). This will give us the compression-tension stress in the wall.
- You can have a play around with how the contours look on screen, have a play around with this to see how it works (I don’t use this option often at all).
- Here you can filter your maximum and minimum stress values. This is very handy, especially for checking cracked regions of the wall, we will look at this in a bit more detail later on. For now I am leaving this as 0 and 0 respectively for Max/Min Range (i.e. no filter).

Here is the resultant appearance of the stress plot on this example shear wall straight out of ETABS (results are in MPa, Megapascal)…

As you can see, there are some high tensions in the base of the wall reducing as the wall increases with height. To make things simpler to determine the cracked regions, we can now use the stress filter outlined previously. We know that our tension capacity of the concrete is 2.8MPa, so we will filter this as our Max/Min range…

Here is what the same stress plot now looks like on that same wall with the stress filter applied…

Blue regions on this plot exceed the 2.8MPa range and therefore this is the region of the wall which is cracked. Regions in purple are lower than 2.8MPa and therefore are uncracked.

The next step is to unlock the model then apply the cracked factor over this region of the wall highlighted in blue. This should be repeated for all shear walls within the building at the same time. For the blue cracked regions here is an example stiffness modifier list taken from ETABS to model the cracked behaviour of this shear wall (note this is in accordance with ACI318 and for a serviceability assessment)…

The model should then be rerun and the stresses re-inspected. It is not uncommon to need to run a few iterations of cracking as cracked walls can lead to more cracked walls within your model (its somewhat of an iterative process, so be prepared to repeat a couple of times).

If you use ETABS frequently and would like to learn some more tips on the software, here are some other articles you may find interesting…

- HOW TO SET UP GRIDS IN ETABS – Sheer Force Engineering
- SHELL VS MEMBRANE, WHICH ONE TO USE IN ETABS – Sheer Force Engineering
- HOW TO CHECK IF YOUR ETABS MODEL IS CORRECT – Sheer Force Engineering
- ETABS oAPI/API TUTORIAL: HOW TO CRACK AUTOMATION SPEED SECRETS USING VBA AND EXCEL – Sheer Force Engineering
- STRUCTURE IS UNSTABLE OR ILL-CONDITIONED: ETABS WARNING FIX – Sheer Force Engineering

## 4 thoughts on “MODELLING CRACKED SHEAR WALL BEHAVIOUR IN ETABS”