[GEN] Automesh and Slab/Wall Design Tutorial

0. Contents 

1. Introduction of Meshed Slab / Wall Design

1-1 Introduction of Meshed Slab / Wall Design

The following design features as per EN1992-1-1:2004 are available in midas Gen.

This tutorial has been provided to explain how to perform meshed slab and wall design. For this reason, the procedure for general frame design process were not included. For the users who are not familiar with the general design features of midas Gen, it is recommended to review “RC Design as per EN1992-1-1:2004” and “Seismic Design for Reinforced Concrete Building” tutorial before going through this tutorial.

1-2 Usage Tip [ Task Pane ]

Using the task pane, we can display work procedure, required input items and optional input items for each analysis and design case. Using the User Defined Task Pane, the user can create a Task Pane manually.
For the meshed slab wall design feature, TDF file was provided with the tutorial model files for the user’s convenience. In order to import the User Defined Task Pane, please follow the procedure below.

1. Go to Task Pane tab in the left panel of the midas Gen window.

2. Click [Task Pane] text from the drop down menu.

3. Click [Import User Defined Page].

4. Select “slab desig.tpd” file and click [Open] button.

1-3 Overview

Typical Floor Plan

Sectional Elevation

1-4 Details of the building

Applied Code

• Eurocode-1:2005

Materials

• Beam : Concrete Grade C25/30

• Column : Concrete Grade C30/37

Girder Section

Column Section

Wall Thickness

Applied Load

2. Model & Automesh

2-1 Opening the pre-generated model file

Open the pre-generated model file.

1. File > Open Project…

2. Select “Meshed Slab and Wall Design_Start.mgb”.

3. Click [Open] button.

2-2 Auto-mesh planar area

Generate meshed elements for slabs

Specify meshed area for auto-meshing (Line elements method).

1. Node/Element > Mesh > Auto-mesh Planar Area

2. Method : Line Elements

3. Type : Quad + Triangle

4. Mesh Size : Length : 0.5 m

5. Material : 1:C25/30,   Thickness : 1:0.2000

6. Domain : 1

7. Select “Select by Plane”

8. Select “XY Plane”

9. Click edge of the ‘Roof’ to select ‘Roof’ as a picture Iso View

10. Click [Apply]

Generate meshed elements for walls

Specify meshed area for auto-meshing (Line elements method).

1. Click > “Select elements by identify”

2. Select “Wall” > [Add]

3. Click [Close]

4. Click [Activation] > [Activate]

Generate meshed elements with opening

Specify meshed area for auto-meshing (Nodes method).

1. Structure > UCS/Plan > UCS > X-Z Plan

2. Origin : 39, 4, 0,   Click : [Apply] > [Close]

3. Structure > UCS/Plan > Grids > Define Point Grids

4. dx, dy : 1, 1,   Click : [Apply] > [Close]

Generate meshed elements for walls

Specify meshed area for auto-meshing (Line elements method).

1. Node/Element > Mesh > Auto-mesh Planar Area

2. Method : Nodes

3. Draw as a picture below.

4. Type : Quad + Triangle

5. Mesh Size : Length : 0.5 m

6. Material : 2:C30/37,   Thickness : 2:0.2500

7. Domain > Name : ‘2’

8. Click [Apply] > [Close]

Generate meshed elements for walls

Specify meshed area for auto-meshing (Line elements method).

1. Method : Planar Elements

2. Type : Quad + Triangle
    Mesh Size : Length : 0.5 m
    Material : 2:C30/37
    Thickness : 2:0.2500

3. Click ‘Select by window’

4. Select as a picture

5. Domain > Name : ‘3’

6. Click [Apply]

Generate meshed elements for walls

Specify meshed area for auto-meshing (Line elements method).

1. Method : Planar Elements

2. Type : Quad + Triangle
    Mesh Size : Length : 0.5 m
    Material : 2:C30/37
    Thickness : 2:0.2500

3. Click ‘Select by window’

4. Select as a picture

5. Domain > Name : ‘4’

6. Click [Apply]

2-3 Define Boundary Condition 

Select all the bottom nodes of model and apply the boundary condition with drag-and-drop function.

1. Click ‘Activate All’ 

2. Toggle off ‘Point Grid’ 

3. Click ‘Select by Plane’  and Select ‘XY Plane’  

4. Select any node at the bottom of model

5. Works Tab in the Tree Menu Click Boundaries > Supports > Type 1 [1111110]

6. Drag & Drop to the model

3. Design Parameters

3-1 Pressure loads

Apply floor loads.

1. Tree Menu > Work > Domain1 [1] > Double Click

2. Load > Pressure Loads

3. Load Case Name : LL

4. Direction : Local z

5. Loads : P1 : -4.0kN/m²
    Shopping areas
    D1 : Areas in general retail shops
6. Click [Apply] > [Close]

Apply floor loads.

1. Tree Menu > Work > Domain1 [2] > Double Click

2. Load > Pressure Loads

3. Load Case Name : LL

4. Direction : Local z

5. Loads : P1 : -2.0kN/m²
    Office areas
6. Click [Apply]

3-2 Building Generation

1. Structure > Building > Control Data > Building Generation

2. Number of Copies : 4

3. Distance(Global z) : 3 m

4. Operations : Click [Add]

5. Check off “Copy Node Attributes” option.

6. Click [Select All] icon 

7. Click [Apply]

3-3 Automatic generation of the story data

1. Structure > Building > Control Data > Story

2. Click [Auto Generate Story Data] button

3. Click [OK]

4. Click [Close]

3-4 Active identity

1. View > Activities > All
    Active Identity

2. Click : Story > 4F

3. Click : [Active] > [Close]

3-5 Define sub-domain

Define sub-domain for design

Reinforcement direction can be specified by sub-domains.

1. Node/Element > Mesh > Define Sub-Domain

2. Click : [2]

3. Rebar Dir.(CCW) : Dir.1 : 135, Dir.2 : 135

4. Click : [Modify] > [Close]

3-6 Wind loads

1. Load > Static Load > Lateral > Wind Loads > Click [Add]

2. Load Case Name : WX
    Wind Load Code : Eurocode-1(2005)

3. Wind Load Direction Factor : X-Dir. : 1, Y-Dir. : 0

4. Click [Apply]

5. Load Case Name : WY
    Wind Load Direction Factor : X-Dir. : 0, Y-Dir. : 1

6. Click [OK]

7. Click [Close]

3-7 Response spectrum functions

1. Load > Seismic > Response Spectrum Data > Response Spectrum Functions

2. Click [Add]

3. Click [Design Spectrum]

4. Design Spectrum : Eurocode-8(2004)

5. Spectrum Type : Horizontal Design Spectrum

6. Click [OK]

7. Click [OK]

8. Click [Close]

3-8 Response spectrum load cases

1. Load > Seismic > Response Spectrum Data > Response Spectrum Load Cases

2. Load Cases Name : RX
    Excitation Angle : 0

3. Check : EURO2004 H-Design

4. Click [Add]

5. Load Cases Name : RY
    Excitation Angle : 90
    > Click [Add]

6. Click [Eigenvalue Analysis control]
    Number of Frequencies : 15
    > Click [OK]

7. Click [Close]

3-9 Automatic generation of load combinations

1. Results > Combination > Load Combination > Concrete Design > Auto Generation

2. Select Design Code as “Eurocode2:04” > Click [OK] > Click [Close]

3. Perform Analysis

4. Frame Design

4-1 Column design

1. Design > Design > RC Design > Design Code

2. Select Design Code as “Eurocode 2:04” > Click [OK]

3. Design > Design > RC Design > Concrete Code Design > Column Design

4. Click [Select All] and then [Update Rebar] button.

5. Sorted by : Member > Check the design results > click [Close]

4-2 Modify column rebar data 

1. Design > Design > RC Design > Modify Column Rebar Data

2. Select SECT “2” in the list.

3. Check the rebar data. Rebar data can be modified in this dialog box.

4. Click [Add/Replace] > [Close]

4-3 Slab and wall load combinations

Slab/Wall Load Combination

Select the load combinations for the slab/wall element design.

1. Design > Design > Meshed Design > Slab/Wall Load Combinations

2. Select the desired load combination in each column to consider during the slab/wall design.

3. Click [OK]

4-4 Design criteria for rebar

Specify rebar size

Enter the standard sizes of rebars used in the design of reinforcement for slab/wall elements.

1. Design > Design Meshed Design > Design Criteria for Rebar

2. For Slab Design : Dir. 1 : 0.03 m, 0.03 m,  Dir. 2 : 0.05 m, 0.05 m

3. Click [OK]

5. Slab/Wall Design

5-1 Active Identity

1. View > Activities > All
    Active Identity

2. Click : Story > ROOF
    Check : +Below

3. Click : [Active] > [Close]

5-2 Slab flexural design

Slab Flexural Design

Check the flexural design results for slab elements in contour.

1. Design > Design Meshed Design > Slab Flexural Design

2. Select [Avg. Nodal].

3. Check [As_req(m^2/m)]

4. Check on One-Way Flexure Design option and click […] button

5. Defined Cutting Lines [Add]

6. Click [Apply]

1. Design > Design > Meshed Design > Slab Flexural Design

2. Select [Avg. Nodal]

3. Click [Design Result]

4. Click [Design Force]

5. Click [Update Rebar]

1. Design > Design > Meshed Design > Slab Flexural Design

2. Check [Resistance Ratio]

3. Load Cases/ Combinations : cLCB5

4. Select [Avg. Nodal].

5. Check [Dir.1]

6. Click [Apply]

[Smoothing]

1. Design > Meshed Slab/Wall Design > Slab Flexural Design

2. Width smoothing : weighted average method

For practical design, smooth moment distributions are preferred. By selecting the smoothing option, the program can consider the smooth moment in slab design.

Element : Design results are displayed using the internal forces calculated at each node of elements.
(no smoothing)

Avg. Nodal : Design results are displayed using the average internal nodal forces of the contiguous elements sharing the common nodes.

Element : Design results are produced for moments at each node of slab elements. (no smoothing)

Width : Design result of slab elements at each node is produced using the average of the bending moments of the contiguous slab elements with the specified width.

(Example) Design force for Node. EN21
In one plate element, 4 internal forces exist. For the element E2, member forces exist at the node EN21, EN22, EN23 and EN24. Following equations show how the smoothing option works for the node EN21. (Assume that rebar direction is selected as Angle 2 for Width smoothing direction.)

(1) Element + Element : EN21

(2) Avg. Nodal +Element : (EN12+EN21+EN33+EN44)/4

(3) Element + Width 2m (dir. 1)

: {(EN21+EN92)*1m/2+(EN21+EN101)*1m/2+(EN21+EN73)*1m/2+(EN21+EN14)*1m/2+(EN21+EN72)*1m/2+(EN21+EN11)*1m/2+(EN21+EN83)*1m/2+(EN21+EN34)*1m/2+(EN21+EN82)*1m/2+(EN21+EN31)*1m/2+(EN21+EN133)*1m/2+(EN21+EN144)*1m/2+(EN21+EN112)*1m/2+(EN21+EN121)*1m/2+(EN21+EN23)*1m/2+(EN21+EN154)*1m/2+(EN21+EN22)*1m/2+(EN21+EN151)*1m/2+(EN21+EN43)*1m/2+(EN21+EN64)*1m/2+(EN21+EN42)*1m/2+(EN21+EN61)*1m/2+(EN21+EN143)*1m/2+(EN21+EN154)*1m/2} /(1m*24)

1. Design > Design > Meshed Design > Slab Flexural Design

2. Check [Wood Armer Moment]

3. Load Cases/ Combinations : CBC : cLCB6

4. Check [Dir.1]

5. Click [Apply]

[Wood Armer Moment]

From the analysis results, following plate forces about the local axis are calculated

- mxx

- myy

- mxy

In order to calculate design forces in the reinforcement direction, angle α and φ will be taken as following figure :

x, y : local axis of plate element
1, 2 : reinforcement direction
α : angle between local x-direction and reinforcement direction 1
φ : angle between reinforcement direction 1 and reinforcement direction 2

Firstly, internal forces (mxx, myy and mxy) are transformed into the a-b coordinate system.

Firstly, internal forces (mxx, myy and mxy) are transformed into the a-b coordinate system.

5-3 Slab shear checking

Slab shear checking

Produce the two-way shear (punching shear) check results at the supports of slab elements or at concentrated loads and the one-way shear check results along the user-defined Shear Check Lines.

1. Design > Design Meshed Design > Slab Shear Checking

2. Click [Apply]

[Punching Shear Check(By Force)]

In this method, the program takes the axial force in the column supporting the slab as the shear force (V_Ed). The basic control perimeter (u1) is taken at a distance 2d from the column face (as shown in the diagram below.

The maximum shear force is calculated by multiplying V_Ed with shear enhancement factor β. The value of β is different for different columns. (as given in the code)

The shear resistance of the slab (without shear reinforcement) at the basic control section is given by
V_Rd,c = (0.18/γ_c)k(100*ρl*fck)1/3*(u1*d) , the value of ρl is assumed to be 0.02.

- V_Ed < V_Rd,c : section is safe in punching shear

- V_Ed > V_Rd,c : provide shear reinforcement.

Asw/sr = (v_Ed-0.75*v_Rd_c)*(u1*d) / (1.5*d*fywd_ef)

[Punching Shear Check(By Stress)]

In these methods (The Stress Method), the Shear force along the critical section is taken and divided by the effective depth to calculate shear stress.

Therefore there is no need to calculate β (Beta), to consider moment transferred to the column.

(There are 4 plate elements intersecting at nodes. The nodes are marked by nomenclature of Grid Lines. As the center node is denoted by B2 , B on x-Axis and 2 on Y-Axis)

When slab is defined as the plate element, the program calculated stresses only at the nodes, in the analysis. So we have the stresses at B1, B2, C2 etc. (see the figure above) are calculated by the program.

Case 1 - To calculate stresses at the critical section that is u1 in the given figure, for example we take the point P in the figure which lies in a straight line. The stress at B1 and B2 are known. The values at these nodes are interpolated linearly to find the stress at point P.

Case 2- Now if the point lies in the curve such as the point Q, then the software will divide the curve into 6 parts. At each point such as Q a tangent which intersects B1-B2 and C2-B2.The value of stresses at T and V are determined by linear interpolation of stresses which are known at for T (at B1 and B2) and for V (at C2 and B2). After knowing stresses at T and V the stress at Q is determined by linear interpolation of stresses at T and V.

(Method 1: Average by elements.)
In this method the stresses at all the critical points is determined. The critical points divide the critical section into segments. The average value for all these segments is determined by dividing the stresses at the two ends of the segment by 2. After determining the average value for each segment, the maximum average value from all of the segments is reported as the Stress value for the critical Section.

a,b are stresses at the segment ends.
Average value for the segment will be (a+b)/2, and such average value for each segment is determined.

(Method 2: Average by Side)
In this method stresses at all critical points is determined and then average stress value is calculated by weighted mean.

To calculate weighted mean , For example we have 4 critical points a, b, c, d.

- Stress at critical points : For example at ‘a’ its 9
- Average of the segment : For example in ‘a’ and ‘b’ its (15+9)/2 = 12
- Distance Between the critical points : For example between ‘a’ and ‘b’ its 8
- Final Stress = (12 * 8 + 17 * 10 + 15 * 6)/ (8+10+6), which is the weighted average.

We divide the Critical section into 4 sides as shown in figure.

The weighted mean value for each side is determined and then the maximum value out of the 4 sides A, B, C, D is reported as the stress value.

5-4 Serviceability parameter

1. Design > Design RC Design > Serviceability Parameter

2. Select All

3. Click [Apply]

5-5 Serviceability load combination type

1. Design > Design Meshed Design > Serviceability Load Combination Type

2. Click [OK] > [Close]

5-6 Slab serviceability checking 

Slab Serviceability Checking

Produce the serviceability check results for slabs.

1. Design > Design Meshed Design > Slab Serviceability Checking

2. Select [Avg. Nodal].

3. Check [Stress Checking]

4. Check [Concrete]

5. Click [Apply]

1. Design > Design Meshed Design > Slab Serviceability Checking

2. Select [Avg. Nodal].

3. Check [Crack control]

4. Check [Crack Width]

5. Select [Value]

6. Click [Apply]

1. Design > Design Meshed Design > Slab Serviceability Checking

2. Select [Avg. Nodal].

3. Check [Deflection]

4. Check [Creep]

5. Select [Value]

6. Click [Apply]

[Stress Checking]

1. Assuming as uncracked section

Calculating σ_conc, σ_steel 

σ_conc = MY/I

σ_steel =(MY/I) * n

2. Verification for uncracked section

Concrete stress

When 'σ_conc > fctm,fl'---> ok

When 'σ_conc < fctm,fl'---> Assuming as cracked section and verification for cracked section is required.

Rebar stress

When 'σ_steel > k3*fyk' ---> ok

When 'σ_steel < k3*fyk' ---> NG

3. Verification for cracked section (if required)

Recalculating concrete and reinforcement stress using Icr :

Concrete stress

When 'σ_conc > k1*fck'---> OK

When 'σ_conc < k1*fck'---> NG

Rebar stress

When 'σ_steel > k3*fyk' ---> OK

When 'σ_steel < k3*fyk' ---> NG

[Crack Control]

1. Crack width

eq(7.8) in EC2-1-1:04

Where, Ap' is considered as zero since it is area of tendon.

2. Min As

Where, σs is a lower value to satisfy the crack width limits according to the max bar size (Table 7.2N) and spacing (Table 7.3N).

3. Rebar Spacing

Refer to the table 7.3N (Maximum bar spacing for crack control).

4. Rebar Dia.

eq (7.6N) in EC2-1-1:04

5-7 Wall design 

Wall Design

Perform the flexural design results for wall elements in contour.

1. View > Activities > Active All

2. Design > Design Meshed Design > Wall Design

3. Select [Avg. Nodal]

4. Select [Resistance Ratio]

5. Click [Apply]

1. Design > Meshed Slab/Wall Design > Wall Design

2. Click [Design Result]

3. Click [Design Force]