ETABS 2016 Analysis of Mat Foundation...Examples utilized: Examples on Page 143 and Page 642;...

ETABS 2016 – Analysis of Mat FoundationAssoc.Prof.Dr. Emre AKIN

Introduction

In finite element analysis, the mat foundation should be meshed into parts which have approximately 1 m2 area. Themultiplication of spring coefficient (ko; unit: kN/m3) and max. vertical displacement (δz,max., found by analysis) willthen give the max. stress under the foundation (σz,max.= ko × δz,max.).

ko→ unit: kN/m3

δz,max. → unit: m

σz,max.→ unit: kN/m2

Check:

σz,max. ≤ σz,allow.

Assoc.Prof.Dr. Emre AKIN

ADU Civil Eng. Dept.

Introduction

The following mat foundation (for a 4-story building) will be modeled and analyzed by using ETABS. The thickness of the mat is selected as 0.80 m. The soil type is hard clay and corresponding modulus of subgrade reaction (ko) is assumed as 20000 kN/m3. The effective depth may be taken as 0.75 m. Materials: C25/S420. Note that cantilever portion of the mat is assumed to have a length of 0.60 m. (away from the column face at all sides). The allowable stress of the soil will be taken as 200 kN/m2.



The analysis was performed considering

column loads corresponding to

«1.4G+1.6Q» combination for the analysis

of building, which yields highest axial

column loads. The axial column loads was

taken from the analysis of 4-story building.

Note: You should take the axial loads of the

columns and shear walls at the ground story

of your own model. Hint: In your own

project, you may distribute the axial loads

of shear walls at the nodes where the the

finite elements of shear wall are joining.Examples utilized: Examples on Page 143 and Page 642; Betonarme

Yapıların Hesap ve Tasarımı; Doğangün, A.

Introduction

The column axial loads at the base which were taken from «1.4G+1.6Q» load combination of the analysis for 4-story building are shown below. The mat foundation will be analyzed for these point loads at the column joints (Load Case: Dead).



Note that each portion between the columns will be

divided into 4×4 parts (meshing). This will provide

approximately 1 m. dimension for each meshed part.

Modeling

Click «File-New Model». In «Model Initialization» window, choose «Display Units» as «Metric SI» under «Use Built-in Settings with:» and click OK! «New Model Quick Templates» window will pop-up. In our example we will have 5 grid lines along both horizontal directions. Let us give a constant spacing of 0.6 m between the grids (we will correct this in the following stage). We have no stories, however we cannot write «0» for the number of stories; so we write «1» here. Fill the appropriate parts as shown below and click OK!



Modeling

The model will be formed where only grids exist. Right click and choose «Add/Modify Grids..». In the following «Edit Story and Grid System Data», click «Modify/Show Grid System». You should correct the «X» and «Y Grid Data» in the «Grid System Data» window as shown below in order to reflect the real distances given three slides before.

Click OK twice when you finish!



Modeling

The grid system should now look as shown below. Go to the «Base –Z=0 (m)» level in the «Plan View» by using «Move Up/Down in List» arrows.



Modeling

Let us define the material in the next stage, by choosing «Define» and «Material Properties». In the «Define Materials» window, click «Add New Material». The «Add New Material Property» window will appear. Here, choose the region as «User», material type as «Concrete» and click OK! You may fill in the values as shown below in the «Material Property Data» and click OK twice!



Modeling

Now we should define the section by choosing «Define», «Section Properties» and «Slab Sections». «Slab Properties» window will appear. Here, click «Add New Property». In the «Slab Property Data» window, choose slab material as «C25» which you defined in the previous stage. You may define the property data as «Mat». Choose «Shell-Thick» members for modeling type. The property data type and thickness should be «Slab» and «800 mm», respectively. Click OK twice!



Modeling

Then choose «Draw», «Draw Floor/Wall Objects», «Quick Draw Floor/Wall» or simply click .Draw the area members starting from the left bottom corner moving to the right each time. Note that section property should be the one that you have defined for the mat (in our case we defined this as «Mat»).

At the end your model should look like as below.You may check, when you right click on any area.



Modeling

Click «Set Display Options» button and activate «Labels» for either joint and shell assignments on «Set View Options» window. After you click OK, the labels for joints and shells will be shown. Here, the order of labels may not be proper.



Modeling

Shell areas F2, F3, F9, F10, F11, F12, F13, F14, F15, F16, F18, F19 will be meshed. The number of meshing along the x and y directions are shown below for each shell label.



Modeling

Activate the shell areas F2, F3, F18 and F19 first by simply clicking on these areas. Then click «Edit» and «Edit Shells» and «Divide Shells». In «Divide Selected Shells» window, choose «Divide Quadrilaterals/Triangles into» as 4 by 1 corresponding to the division operation along x and y directions.



Modeling

Repeat the same operation for all similar shell areas by using proper numbers of division along the x and y directions as given in the table (two slides before). At the end your model should look like this. In order to arrange order of labeling properly, choose «Edit» and «Auto Relabel All». It will ask you that this operation cannot be undone; click «Yes» for this. Now all labels should be in an order starting from the bottom left corner as shown below.



Modeling

Our shell members are only expected to bend about the horizontal x and y directions (in plan) and translate along the vertical z-direction when subjected to out-of-plane loads (loads along the z-direction). Therefore, we will define support conditions at the bottom of our model to eliminate the translational degrees of freedom in plan (along x and y-directions) and rotation about z-axis (twist). In order to do this, select all your model first (Ctrl+A). Then choose «Assign», «Joint» and «Restrains». In the «Joint Assignment» window, activate restraints for «Translation X», «Translation Y» and «Rotation about Z». Click OK!



Modeling

We should also define springs under the shell areas to reflect the resistance of soil under the mat foundation when shell members are subjected to out-of-plane loads and displace along the z-axis. The spring coefficient should be 20000 kN/m/m2 (modulus of subgrade reaction, ko). In order or to define the springs under shell members, choose all your model (Ctrl+A). Then, choose «Assign» «Shell» and «Area Springs».



Modeling

Then, click «Modify/Show Definitions» on «Shell Assignment-Area Springs» window. The «Area Spring Properties» window will pop-up. Here, select «Add New Property». In the following «Area Spring Property Data» window, it is important to write 20000 kN/m/m2 for spring constant corresponding to local 3 direction (others should be zero). You may choose not to change property name. Click OK three times!



Modeling

Next we should apply the vertical point loads transferred by the columns (axial loads corresponding to «1.4G+1.6Q» load combination). These loads and the joint label for each load are shown in the table below.



First select the joint where the load is to be applied (start selecting joint «13»). Then choose «Assign», «Joint Loads» and «Force». In the following «Joint Load Assignment-Force» window, write «-403.60» kN for the «Force Global Z». This will apply 403.60 kN vertical downward load at joint 13. «Load Pattern Name» may remain as «Dead». Repeat the same procedure to apply loads to the other joints as given in the table.

Joint 13 should be selected first!

Modeling

At the end, if you choose «Display», «Load Assigns» and «Joint» when the 3-D screen is selected, you should see the applied loads as shown below.



Analysis Results&Design

• At the final stage, save the project and run the analysis. • In order to see the vertical displacements (settlement), choose «Display», «Deformed Shape». On «Deformed

Shape» window, choose «Draw contours on objects». Contour component should be «Displacement UZ» (vertical displacement along z-axis). You should see the change of settlement on the mat foundation area in x-y view (following figure).



The maximum settlement is at the top left corner, whichis (δz,max.) 4.596 mm. (negative, in the downwarddirection). The maximum stress:

𝜎𝑧,𝑚𝑎𝑥. = 𝑘𝑜 × 𝛿𝑧,𝑚𝑎𝑥. = 20000𝑘𝑁

𝑚3 × 0.004596

= 91.92𝑘𝑁

𝑚2 < 200𝑘𝑁

𝑚2 SAFE!


In order to see the distribution of bending moment about y-axis, choose «Display», «Show Force/Stress Diagrams», «Shell Stresses/Forces». On «Shell Forces/Stresses» window, choose «M11» as «Component». The reinforcement along x-direction will be determined based on this bending moment. Due to positive moment, there will be tension at the lower side of the foundation. Due to negative bending moment, there will be tension at the upper side of the foundation.



Therefore you may determine the bottom and top

reinforcement (along the x-direction) by considering

highest negative and positive bending moments (about

the y-axis), respectively.

𝐴𝑠,𝑏𝑜𝑡𝑡𝑜𝑚 =𝑀𝑑+

𝑓𝑦𝑑×𝑗𝑙×𝑑

𝐴𝑠,𝑡𝑜𝑝 =𝑀𝑑−


As an example, the demonstrated analysis has the

highest negative bending moment about x-axis with a

value of -135.08 kN.m/m (as shown in the next figure).

+M11Local Axis 1

Loca

l Axi

s 2

Note: You may check the local axes of shell members by choosing «Set Display Options». Then on «Object Assigments» menu, «Shell Assignments», «Local Axes» should be activated. On the model, red and green axes correspond to axis 1 and axis 2, respectively.


In order to see the distribution of bending moment about x-axis, choose «Display», «Show Force/Stress Diagrams», «Shell Stresses/Forces». On «Shell Forces/Stresses» window, choose «M22» as «Component». The reinforcement along y-direction will be determined based on this bending moment. Due to positive moment, there will be tension at the lower side of the foundation. Due to negative bending moment, there will be tension at the upper side of the foundation.



Therefore you may determine the bottom and top

reinforcement (along the y-direction) by considering

highest negative and positive bending moments (about

the x-axis), respectively.

𝐴𝑠,𝑏𝑜𝑡𝑡𝑜𝑚 =𝑀𝑑+


𝐴𝑠,𝑡𝑜𝑝 =𝑀𝑑−


As an example, the demonstrated analysis has the

highest negative bending moment about x-axis with a

value of -138.98 kN.m/m (as shown in the next figure).

+M22

Local Axis 1

Loca

l Axi

s 2

Note: You may check the local axes of shell members by choosing «Set Display Options». Then on «Object Assigments» menu, «Shell Assignments», «Local Axes» should be activated. On the model, red and green axes correspond to axis 1 and axis 2, respectively.


• The shear capacity-demand check should also be done. The shear forces (demand) that will be taken into account are V13 and V23 according to the definitions of ETABS.



«Display», «Show Force/Stress Diagrams», «ShellStresses/Forces». On «Shell Forces/Stresses» window,choose «V13» (and then «V23») as «Component».Check the maximum of any V13 or V23 values andtake this maximum value as Vd. In our model, Vd=121kN. The shear force capacity for cracking (on b=1m=1000 mm width):𝑉𝑐𝑟 = 0.65 × 𝑓𝑐𝑡𝑑 × 𝑏 × 𝑑 = 0.65 × 1.2 × 1000 × (800 − 50)

𝑉𝑐𝑟 = 585000N = 585 kN > 𝑉𝑑 = 121 𝑘𝑁 SAFE!

Clear cover for foundation:d’=50 mmfctd=1.2 MPa for C25

Analysis Results&DesignAssoc.Prof.Dr. Emre AKIN


The mat foundation is reinforced by longitudinal bars at the upper and lower portions of the foundation, alongboth x- and y-axis (mesh type reinforcement). These longitudinal reinforcements are calculated regarding thebending moments, as explained in the previous slides. The free edges of the foundation is reinforced by hairpinbars (no calculation). The upper reinforcements are held in place by means of rebar chairs (no calculation). Theadditional punching reinforcement against punching (if required) is as follows:

Reference: Website «http://debug.pi.gr/Default.aspx?ch=77»

ETABS 2016 Analysis of Mat Foundation...Examples utilized: Examples on Page 143 and Page 642;...

Documents

Transcript of ETABS 2016 Analysis of Mat Foundation...Examples utilized: Examples on Page 143 and Page 642;...