# Earthquake Analysis with RSA¶

This tutorial explains the workflow for an earthquake analysis using the Response Spectrum Analysis (RSA).

## Introduction¶

The following Tutorial describes the general workflow of the task Earthquake. Guided by the Earthquake task , all necessary input will be defined. The focus of these calculations is based on the Elastic Response Spectra method. For further information we refer you to our handbooks DYNA_1.pdf and DYNR_1.pdf and to further technical literature.

Note

A basic SOFiSTiK knowledge is required for this tutorial. This tutorial is based on program version 2016.

You will find the data files on our ftp-server.

Note

You need the current SONAR login and password to get access to the files.

The SSD-Task Earthquake uses the linear elastic Response Spectra Method. For further information please read the corresponding literature. The following explanations describe the SSD-task Earthquake and the necessary input. Add the task to your project and open it with a double click. The dialogue contains 8 tabs, whereas 3 tabs are for the definition of the response spectra in x-, y- and z-direction. The tabs are shortly introduced in the following chapters. After all tabs are filled out you close the dialogue with the “OK” button. Usually the option “Process immediately” is set. That means with clicking “OK” the analysis starts right away.

Note

Generally, the default settings given are sufficient for calculation. The resulting load cases will be saved automatically as part of the action E...Earthquake. Later on in the analysis you can easily refer back to these load cases.

In case you want to see the text input, created automatically by the task, you use the context menu with the right mouse click on this task and select the command “Text Editor”.

Warning

Any changes made manually inside this text input file will be overwritten if the dialogue is subsequently opened and closed by clicking “OK” button.

Note

Random torsion moments are not available within the Earthquake task. If this is required, input can be made via manual text entry using TEDDY or by converting the Earthquake task into a User Task

### Tab Eigenvalues¶

Definitions for calculation of Eigenvalues. The default settings are generally sufficient for a range of projects. For further information, please refer to the DYNA handbook.

### Tab Damping¶

Input for damping is entered here. Modal damping is generally sufficient. For normal buildings the damping values are usually between 3% and 5%. In the Expert settings, a damping value can be defined for each Eigenvalue.

### Tab Additional Masses¶

Additional masses can be defined here. The structures self-weight will be taken into account automatically. In addition, one can convert load cases into masses. In the default settings, all load case factors will be converted into masses at a value of 100%. Specific percentage and direction settings for conversion of load cases into masses are also available.

Warning

In cases where self weight and dead loads are saved in the same load case, only the self weight will be converted to masses. For that reason we recommend to use a separate load case for self weight only and another for dead loads.

### Tab Directions of Action¶

Definition of directions of actions. In most cases the calculation of horizontal directions only is sufficient. Using the Expert settings more specific definition can be made. For example, the acceleration can be applied only to selected groups.

### Tab Response Spectra (horizontal directions)¶

Defines the Response Spectra according to the selected code, soil class and seismic zone. A graphical control for direct entry is available.

### Tab Results (Text Output)¶

Defines the superposition method of Modal Results. We generally recommend using the CQC Complete Quadratic Combination method. It is important to define separate load case numbers for every result, like the default settings.

Warning

If duplicate load case numbers are used, the results of previous calculations will be overwritten.

## Tutorial Example Earthquake Calculation¶

Please see the following project information before starting to set up your project files.

### Materials¶

Number Material Strength
1 concrete C 20/25
2 reinforcement steel S 500

### Cross Sections¶

Element Dimension Weight
Column B/H = 30/30 cm g = 0,225 t/m
T-Beam B/H/Bw/Hf = 70/60/30/20 cm g = 0,300 t/m (w/o slab flange)
T-Beam, edge B/H/Bw/Hf = 50/60/30/20 cm g = 0,300 t/m (w/o slab flange)
Slab D = 20 cm g = 0,500 t/m²

### Geometry¶

LC Number Title Loads
1 Dead Load g1 = 1,50 kN/m² (100% mass active)
2 Live Load q2 = 2,00 kN/m² (15% mass active)
3 Live Load Roof q3 = 3,00 kN/m² (30% mass active)
10 structure self weight automatic generation “Factor of dead weight” = 1.0

The following picture shows the loads and load cases on the structure.

## Start New SSD Project¶

To start a new project please open the SSD and go to menu “File” > “New Project”. Now the “System Information” dialogue opens. Please define project title, project name and project directory first.

Note

We recommend to use a local directory for your project files to speed up communication between program and data base. Later on you can zip and save your project data on a company server.

Now select the code. First select the country flag and then the code. In case you like to use the pure Eurocode without any national annex use the European flag. For further Information about available design checks please read the manuals AQB and BEMESS chapter NORM.

Warning

If you leave the “System Information” dialogue with “OK” the selected country code is fixed and saved inside the data base. You may NOT change the code later on.

With the orientation of the dead load you define the global coordinate system. We are using a red arrow for the x-direction, a green arrow for the y-direction and a blue arrow for the z-direction. These colours will be used in all our program modules.

Working with SOFiPLUS you have two major options:
• working with structural elements (automatic mesh generation)
• working with finite elements (manual meshing)

Warning

You must select one option to generate your system. A mix of both methods is not allowed in the graphical input, but can be done with script language inside TEDDY.

Warning

If you leave the “System Information” dialogue with “OK” the global coordinate direction is fixed and saved inside the data base. You may NOT change the direction later on.

## Material Definition¶

Inside the SSD task-tree the task “Materials” is one of the default settings.

Simply use the right mouse click function to generate as many new materials as necessary.

Note

In case you have different construction stages in your cross section (e.g. composite section), it is necessary to define separate materials for every stage even if the material properties are the same for both parts.

Extra material constants may be defined for any type of material (AQUA:MEXT record). Please refer to AQUA manual for more details:

## Cross Section Definition¶

Inside the SSD task-tree the task “Cross Sections” is one of the default settings.

Few options are available:

• Cross-section-values
• Plate
• Rectangle
• T-Beam section
• Circle / annular section
• Tube
• Cable section
• Rolled steel

Hint

Simply use the right mouse click function to generate as many standard cross sections as necessary. Specific bridge cross sections will be generated later via SOFiPLUS - Cross Section Editor.

Using the context menu with the right mouse click you can create new cross sections. For this example we require three new standard cross sections. For the dimensions and materials see table above.

## System- and Load Definition with SOFiPLUS(-X)¶

The system and load generation will be done with SOFiPLUS(-X). T-Beam section #3 will be applied along all slab edges, and T-Beam section #2 for all other beams. We strongly recommend to use the provided template drawing for generating the system. In the data files directory available for download alongside this tutorial, you will find a drawing titled “only_dwg_earthquake_multistorey.dwg” which can be used to get started.

Note

Slabs, beams and columns should be defined according to their center of gravity. It is necessary to divide the columns vertically into multiple elements to better consider their mass distribution. The option “create regular (rectangular) mesh if possible” should be used for the structural areas because all columns are defined by specific structural points at the beginning or end of structural lines.

Warning

Define self weight within a single load case #10 without any additional dead loads.

## Analysis of Single Load Cases¶

The calculation of individual load cases is done by using the task “Linear Analysis”. Select the option “Process immediately”, which starts the analysis after finishing the input with OK. Additional input inside the dialogue is not necessary. Usually you may switch off all standard generated graphics from the tab “Graphical Output”. To display loads and results a new task “Interactive Graphic” will be added to the project. Open this task and create all the result plots you want to have.

## Insert Task Earthquake¶

With a right mouse click in the Task Tree you open the context menu. Select the command “Insert Task” and select the task “Earthquake” from the task library. Confirm the selection with OK. Now a new task “Earthquake” will be added to the project. For that we recommend to create a new group called “Earthquake” and drag this new task inside the group. The necessary input follows the description given in chapter SSD-Task Earthquake.

### Step 1: Tab Eigenvalues¶

According to the rule of Eurocode 1998 it is necessary to have more than 90% of all masses active. Therefore the number of eigenvalues depends on that rule. As a standard procedure you simply run this task and check the results. In case less than 90% of the masses are active you need to increase the number of eigenvalues. The necessary settings are shown in the following picture.

### Step 2: Tab Damping¶

In any case you have a damping in your structure. Usually a modal damping of 5% will be used. In case of steel structures the damping values may be smaller.

### Step 3: Additional Masses¶

Loads which act permanently on your structure should be transferred into masses as well. The self weight of the structure is transferred into masses automatically. Loads which are defined in the same loadcase as the structure self weight will NOT be converted into masses. That’s the reason, why we recommend to use a separate load case for the structure self weight. Inside the dialogue all available load cases are listed in a table. Now you can select, whether all loads (column “Convert All”) or only parts of the loads should be converted into masses. In the latter case simply untick the option “Convert All” and tick the direction of the load. In general you want only vertical loads to be converted into masses. Therefore you have to tick “LC to z”.

Converted masses will act usually in all three directions. Therefore the percentage value of the converted masses must be set with the same value in x-, y- and z-direction.

Note

Inside the table there is a column “Psi2”. This values has no effect on the input. It is only an additional information for the user. The value psi-2 represents the combination factor of a permanent combination.

### Step 4: Directions of actions¶

Based on the rules of the code it may be necessary to have different spectra for horizontal and vertical directions. If so, you have to select these options here. Usually you will use only one spectrum for both horizontal directions and neglect the vertical directions.

In case parts of the structure should not be used for the analysis, the corresponding group of elements can be selected and activated here as well.

### Step 5: Response Spectra (horizontal directions)¶

The most important step is the definition of the response spectrum. The user may select from a list of different standard response spectra. According to the Eurocode two types of response spectra are possible. The selection EC-1 refers to type 1 and EC-2 refers to type 2. Another option is the selection between “Elastic-Spectra” and “Design Spectra”. The difference is, that the values of the design spectrum are the values from the elastic spectrum divided by a behaviour factor q. Usually this factor is set to q = 1.5. In case the user selects a “Design Spectra”, the behaviour factor and all further values to define the spectrum are set automatically. For that reason a manual input in the area “Expert Settings” is not necessary, except the selection of the Soil Class. The last important inputs are the “Acceleration” and the “Factor horizontal”. The acceleration is based on the location of the structure and is given by the code. The horizontal factor is used as the importance factor from the code. That means the final acceleration used in the analysis is the product of acceleration * Factor horizontal. In our example we will use the following settings:

Response Spectrum according Eurocode Type 1 --> EC-1
Elastic Spectra
Acceleration      Ag = 0.8 m/s²
Factor horizontal Ah = 1.0
Soil Class        A


Inside the dialogue the response spectrum curve is plotted. As soon as the user changes the input values the curve will be updated. This enables the user very easily to check the input data. If the user clicks on one edit field in the “Expert Settings” area, the corresponding value will be shown in red colour inside the plot

### Step 6: Results (Text Output)¶

This last step organises only the required results. Based on the modal analysis, which is the background of the elastic response spectrum analysis, the superposition method for all single modes must be set first. Usually we recommend to use the CQC - Complete Quadratic Combination method. This is also the default setting. Next the required result load cases for nodes, beam and shell elements must be set. Please ensure that the result load cases have not been used before and are not used again after this analysis. All result load cases will be saved into the Action E - Earthquake. In case this action is not already defined in the project file, the program will automatically define this action. Later on all load cases from this action will used in one selection for further superpositionings.

For the final results from the response spectra analysis there are two combinations necessary. The first one is the combination of the different modes. This option is set with the selection of “Default Superposition Method of Modal Results”. The second one is a combination of the two main directions. As defined in step 5, we do have two major earthquake directions. The modal analysis will be performed separately for every direction. After that a combination is performed automatically using the SRSS method (SRSS = Square Roots fo Sum of Squares). This is possible following the rules of Eurocode 1998.

Note

All necessary combinations including the main directions will be done automatically. A separate and manual defined combination of 100% Ex + 30% Ey is not necessary according to EN 1998-1, chapter 4.3.3.5.1 (2) rule b). The combination of the directions cannot be changed within the dialogue. This can be done manually inside the text editor, but is not recommended.

After finishing all input, close the dialog with the “OK” button. Usually the option “Process immediately” is ticked and the program starts the analysis right away.

Warning

Based on the modal analysis procedure results will be generated independently for every single element. Therefore we will not get corresponding results for neighboured elements.

### Step 7: Check In- / Output in Report Browser¶

After performing the Response Spectra Analysis it is very important to check either the automatic generated input as well as the results inside the report browser. To check the input use the context menu command “Text Editor” from the right mouse click on task “Earthquake”. A sequence of three program modules was generated automatically: PROG SOFiLOAD, PROG ASE and PROG DYNA. These modules represent the definition of the response spectra, separated for the two main directions, the eigenvalue analysis and the evaluation of the response spectrum analysis.

The input sequence is printed below:

+PROG SOFILOAD urs:15 $Definition Response Spectra HEAD Definition Response Spectra PAGE UNII 0 LC 990 TYPE NONE RESP TYPE EC-1 CLAS A MOD 1.500 SA 0.670 SB 1.667 SMIN 0.200 TB 0.150 TC 0.400 TD 2.000 TE 0.0 K1 1.000 K2 2.000 AG 0.4 AH 1.0 ACCE DIR Ax 1 LC 991 TYPE NONE RESP TYPE EC-1 CLAS A MOD 1.500 SA 0.670 SB 1.667 SMIN 0.200 TB 0.150 TC 0.400 TD 2.000 TE 0.0 K1 1.000 K2 2.000 AG 0.4 AH 1.0 ACCE DIR Ay 1 END +PROG ASE urs:15.1$ Calculation Of Eigenvalues
HEAD Calculation Of Eigenvalues
PAGE UNII 0
CTRL OPT SOLV VAL - $Solution of the system MASS FACT MZ 0.001 MASS 0 MASS -1 MASS -30002 MX 0.015 MY 0.015 MZ 0.015 MASS -30003 MX 0.03 MY 0.03 MZ 0.03 CTRL MCON 3 EIGE NEIG 10 ETYP LANC NITE - MITE - LC 9001 END +PROG DYNA urs:15.2$ Calculation of Spectras
HEAD Calculation of Spectras
PAGE UNII 0
CTRL STYP 3
EIGE NEIG 10 TYPE REST LC 9001
MODD (1 10 1) 5.000/100
LC  990
LC  991
EXTR U 981 STYP CQC ACT E $Node - Displacement is saved in loadcase 981 EXTR V 982 STYP CQC ACT E$ Node - Velocity is saved in loadcase 982
EXTR A 983 STYP CQC ACT E $Node - Acceleration is saved in loadcase 983 EXTR N 901 STYP CQC ACT E$ Beam - Normal force is saved in loadcase 901
EXTR VY 902 STYP CQC ACT E $Beam - Shear force Vy is saved in loadcase 902 EXTR VZ 903 STYP CQC ACT E$ Beam - Shear force Vz is saved in loadcase 903
EXTR MT 904 STYP CQC ACT E $Beam - Torsional moment is saved in loadcase 904 EXTR MY 905 STYP CQC ACT E$ Beam - Bending moment My is saved in loadcase 905
EXTR MZ 906 STYP CQC ACT E $Beam - Bending moment Mz is saved in loadcase 906  The next thing to check is the sum of loads and the converted masses. The results are printed in two different positions inside the report. The first time you will see an output with “Sum of Masses” form the module ASE. Second you will see an output of “Sum of Masses” from module DYNA. As you see, there is a difference in the results. Before we check the masses by hand calculation we go into the SSD window and check the result tables, tab “Results”. You see the sum of loads for each load case. The sum of loads from LC 1,2 and 3 will be used together with the percentage (convert load to masses) value. The masses printed from the module DYNA are shown in the following picture: If you add the masses you can easily reproduce the sum of masses printed from the module DYNA [1]: self weight only: 212,625 + 273,000 = 485,625 [t] self weight + 10% LC 1 + 15% LC 2 + 30% LC 3: 485,625 + 1,00*819,0/10 + 0,15*624,0/10 + 0,30*728,0/10 = 598,725 [t]  The masses printed from the module ASE are shown in the following picture: If you add the masses you can easily reproduce the sum of masses printed from the module ASE [2] [3]: self weight only: If we take away the flanges of the T-beam sections we get: 212,625 - (13*6.5+13*4.0)*0.2*0.7*25/10 - (16*6.5+16*4.0)*0.2*0.25*25/10 + 273,000 = = 212,625 - 47,775 - 21,000 +273,000 = 416,850 [t] self weight + 10% LC 1 + 15% LC 2 + 30% LC 3: 416,850 + 1,00*819,0/10 + 0,15*624,0/10 + 0,30*728,0/10 = 529,950 [t]  This is based on the fact, that the module ASE takes care of the overlapping of weight and stiffness between T-beam section and slab. The module DYNA is not able to do so. To check the masses simply add a new task “Summary of Masses” from our task library to your project and run this task. The results are printed in tables organised by the element group number. It should be clear from the above that our recommendation is to use the module ASE for the eigenvalue analysis. There is still a small difference between the total masses and active masses values. This is based on the fact, that all masses will be applied in the nodes of elements. As we do have rigid supports for our columns, the masses in this nodes cannot be active for any Eigenvalue. That’s the reason, why the active masses are a little smaller than the total masses. With the next check we will have a look at the Eigenfrequencies. You will find a table output from module DYNA. Most important is to check, whether the total modal mass is greater than 90% of the active mass. In our case we have a modal mass from 99.1% and everything is fine. In case you have a value less than 90% you have to increase the number of Eigenvalues. Note In case you do have a raft foundation, you never can fulfil the 90% rule of modal masses. This is based on the fact that the raft foundation has a huge mass, but this mass is not active. This happens usually if the raft is modelled as a slab with a bedding constant. As a workaround you may define the raft with a special concrete with gam=0.0 and the self weight of the concrete is applied by a separate loadcase to the structure. ## Define Combinations and Superpositions¶ Using the default settings, combination rules are created automatically according to the selected design code. If you start the task “Define Combination” after analysing the task “Earthquake” the necessary combinations will be generated automatically. In case it will be necessary to create a new earthquake design combination “Ultimate Limit State Earthquake” open the task “Define Combinations”, select “Insert new element”, and select “Ultimate Earthquake combin. ” . For the superposition “Kind” and “Type of Resulting Loadcases” choose “Semi-automatic” resulting loadcases. Select the new “Ultimate Earthquake Combination” and add the required actions and load cases. Use the option “Add the most unfavourable with unfavourable sign (x1-X99)” for the result load cases from earthquake analysis. All selections will be done on the right hand side of the dialogue. Save the input by using the “<<” button to move the information to the tree on the left hand side. Finally the settings will be saved directly into the database *.cdb when closing the dialogue with the “OK” button. For more information please see our MAXIMA manual chapter 4. We recommend to eliminate the option “Supporting Forces in Nodes” for the earthquake superposition. Based on the analysis procedure, we do not generate any support forces. Therefore it makes no sense to generate a superposition including support forces. All resulting loadcases will be saved as type “Ultimate Earthquake Combination”. This makes the following design process much easier, because the selection of all design load cases will be only by type of loadcase. Opening the report browser you will see the following output. Checking the analysis results you will see a long list of warnings. These warnings are all correct and of no concern. The reason why is easy to explain. All results of the earthquake analysis are saved in one action E...Earthquake. If we do the superpositioning for a QUAD element including all loadcases saved in action E, the program tries to combine loadcases with beam results and with QUAD results. Of course this is not possible. Therefore the warning tells you, that a specific loadcase, e.g. containing only beam results, does not contribute anything to the superpositioning. The warning is shown below. Now we can proceed with the design process. ## Design Elements¶ ### Standard Procedure¶ For the design, some new tasks need to be added to the Task Tree. Please add the following tasks by using the command “Insert Task” from the context menu with the right mouse click. • ACCI- area elements (Earthquake) • ULS- beams • ACCI – beams (Earthquake) For a better organisation you may use the command “Insert Group” from the context menu with the right mouse click and add a group “Design Beam Elements” The design of area elements follows the principles described in the SSD/SOFiPLUS introduction. In this example only the more important concepts for ultimate state earthquake design are described in more detail. Basically the task “Design ACCI - Area Elements” and “Design ACCI - Beam Elements” work similar. A new design case to store the necessary reinforcement will be defined. Usually this will be design case 11. The task will automatically select all combined load cases of type “Earthquake Combination”. The user can simply use the default settings and run the tasks. Usually we do not use the automatic generated plots and use a new task “Interactive Graphic” to set up all necessary plots. Note After finishing the design process, you must combine the necessary reinforcement from different design cases. This must be done by an additional task. “User Text” The input sequence is printed below: +prog bemess urs:37.1 head Combine Design Results QUAD CTRL LCRI 1,11$ take results from distribution 1 and 11
CTRL LCR 20             $accumulate both results and save maximum in distribution 20 end +prog aqb urs:37.2 head Combine Design Results BEAM rein rmod accu lcr 1$ take results from distribution 1
rein rmod accu lcr 11   $take results from distribution 11 rein rmod sing lcr 20$ accumulate both results and save maximum in distribution 20
end


The final plot of the necessary beam reinforcement in the building axis is shown in the picture below.

### Change Safety Factors¶

According to the code EN 1998-1, chapter 5.2.4 (2), the user must change the safety factors for concrete and steel back to the persistent and transient safety factors. To achieve that in our input file, the user must convert the SSD-tasks “Design ACCI - area elements” and “Design ACCI - beam” into a user task. After this is done please make the following changes to the tasks:

+PROG BEMESS $ULS design acci - QUAD - new safety factors HEAD ULS design acci - QUAD - new safety factors PAGE UNII 0 CTRL ACCI CTRL LCR 11$ Reinforcement distribution number
CTRL RO_V 0.20                    $Maximum reinforcement for shear for normal slab region MAT sc1 1.5 sc2 1.5 ss1 1.15 1.15$ Change safety factors
PUNC NO
LC EARQ
END

+PROG AQB  $ULS design acci - BEAM - new safety factors HEAD ULS design acci - BEAM - new safety factors PAGE UNII 0 BEAM TYPE BEAM REIN MOD SECT RMOD SING LCR 11$ Reinforcement distribution number
DESI STAT ACCI sc1 1.50 sc2 1.5 ss1 1.15  $Change safety factors LC TYPE (E) END  The next figure shows a clipping from the EN 1998-1 code. ## Accidental Torsional Effects¶ According to EC 8 or DIN 4149 you should consider accidental torsional effects for every floor. A dialogue based input via SSD is not yet available, therefore a manual input is necessary. The first step is to convert the Earthquake task into a user defined task. This is not a reversible action done with the command “Convert to User Task” from the context menu after a right mouse click. Now you are able to edit the input generated by the program manually. For the following tasks a basic knowledge of TEDDY and the CADINP input language will be required. All relevant input for the accidental torsional effect will be done in PROG SOFiLOAD, following the ACCE function. Warning To use the additional forces due to accidental torsional effect, it is necessary to change the order of program modules as follows: • PROG ASE$ Analysis of Eigenvalues
• PROG SOFiLOAD $Definition Response Spectrum + torsional eccentricity • PROG DYNA$ Response Spectra Analysis

This order is very important because nodal masses are needed to calculate forces according to the accidental eccentricity. For further explanation refer to the manual SOFiLOAD_1.pdf, Section 4.4 ACCE – Accelerations. Use a separate ACCE input line for every floor. The literal REFX or REFY define the eccentricity referenced to the center of mass. With the literals XMIN, YMIN, ZMIN, XMAX, YMAX and ZMAX you define a selection box to cover the relevant floor. Inside the ACCE sentence you must change the input ACCE DIR into ACCE DIRN.

Note

The eccentricity is always acting perpendicular to the main earthquake direction. The correct input is similar to:

ACCE DIRN AX 1.0 REFY ...
and
ACCE DIRN AY 1.0 REFX ...


Warning

The following input file uses a CADINP feature to extent the input into the next following line. The first line of the ACCE record shown below ends with an double-dollar-sign and will be followed by the next input line. If you forget the double-dollar-sign, you will define a wrong selection box, which will give wrong results. The correct input looks like:

ACCE DIRN Ay 1 REFX -0.05*19.2  XMIN   -1.0 YMIN  -1.0 ZMIN  -5.0 $$XMAX 20.0 YMAX 13.0 ZMAX -2.0  The following input shows the basic workflow according to this tutorials example:  First do the Eigenvalue Analysis to get nodal masses  for torsional forces; masses are saved in the central data base +PROG ASE urs:15.1  Calculation Of Eigenvalues HEAD Calculation Of Eigenvalues PAGE UNII 0 CTRL OPT SOLV VAL -  Solution of the system MASS FACT MZ 0.001 MASS 0 MASS -1 MASS -30002 MX 0.015 MY 0.015 MZ 0.015 MASS -30003 MX 0.030 MY 0.030 MZ 0.030 CTRL MCON 3 EIGE NEIG 10 ETYP LANC NITE - MITE - LC 9001 END  Definition of eccentricities for accidental torsional moments +PROG SOFILOAD urs:31.1  Definition Response Spectrum HEAD Definition Response Spectrum ECHO LOAD EXTR LC 990 TYPE NONE RESP TYPE EC-1 CLAS A MOD - SA 1.000 SB 2.500 SMIN 0.0$$
TB 0.150 TC 0.400 TD 2.000 TE 0.0 K1 1.000 K2 2.000 AG 0.4 AH 1.0
$accidental eccentricity$ Li..floor dimension perpendicular to the direction of seismic action
$1. Floor Ly 12.0 m ACCE DIRN Ax 1 REFY +0.05*12.0 XMIN -1.0 YMIN -1.0 ZMIN -5.0 $$XMAX 20.0 YMAX 13.0 ZMAX -2.0 2. Floor Ly 12.0 m ACCE DIRN Ax 1 REFY +0.05*12.0 XMIN -1.0 YMIN -1.0 ZMIN -8.5$$ XMAX 20.0 YMAX 13.0 ZMAX -5.5$ Roof     Ly 8.0 m
ACCE DIRN Ax 1 REFY +0.05*8.0   XMIN   -1.0 YMIN  -1.0 ZMIN -12.0 $$XMAX 20.0 YMAX 13.0 ZMAX -9.0 LC 991 TYPE NONE RESP TYPE DIN CLAS B-T MOD 0.050 SA 1.000 SB 2.500 SMIN 0.0$$
TB 0.100 TC 0.300 TD 2.000 TE 0.0 K1 1.000 K2 2.000 AG 0.8 AH 1.2
$accidental eccentricity$ Li..floor dimension perpendicular to the direction of seismic action
$1. Floor Lx 19.2 m ACCE DIRN Ay 1 REFX -0.05*19.2 XMIN -1.0 YMIN -1.0 ZMIN -5.0 $$XMAX 20.0 YMAX 13.0 ZMAX -2.0 2. Floor Lx 19.2 m ACCE DIRN Ay 1 REFX -0.05*19.2 XMIN -1.0 YMIN -1.0 ZMIN -8.5$$ XMAX 20.0 YMAX 13.0 ZMAX -5.5$ Roof     Lx 13.0 m
ACCE DIRN Ay 1 REFX -0.05*13.0  XMIN   -1.0 YMIN  -1.0 ZMIN -12.0 
XMAX   20.0 YMAX  13.0 ZMAX  -9.0
ENDE

$Now start calculation of Spectras +PROG DYNA urs:31.3$ Analysis of Response Spectra
HEAD Calculation of Spectras
CTRL STYP 3
EIGE NEIG 10 TYPE REST LC 9001
MODD (1 10 1) 5.000/100
LC  990
LC  991
EXTR U 981 STYP CQC ACT E $Node - Displacement is saved in loadcase 981 EXTR V 982 STYP CQC ACT E$ Node - Velocity is saved in loadcase 982
EXTR A 983 STYP CQC ACT E \$ Node - Acceleration is saved in loadcase 983
...
ENDE


Please use WINGRAF to check the effect of the accidental torsional effects. Select the LC 990 and 991 and display the element related loads.

Based on the input ACCE DIRN the program generates nodal forces including the additional torsional effects. The general principles will be explained according the following little examples. We look at a simple table structure of 10,0 m x 12,0 m with no masses except 4 nodal masses of 5[t] each in the top corner nodes. The base acceleration is set to:

$a = 0.84 \ [m/s²]$

And the eccentricity is set to:

$e = 0.05 \cdot 12.0 = 0.6 \ [m]$

The additional acceleration is computed to:

$\frac {\partial a}{\partial r} = e \cdot a \cdot \frac{{\sum m_i}}{\sum {m_i \cdot r^2_i}} = 0.06 \cdot 0.84 \cdot \frac {4 \cdot 5}{4 \cdot 5 \cdot 5.61} = 0.0083 \ [1/s²]$

The additional forces are computed to:

$F_i = \frac{\partial a}{\partial r} \cdot m_i \cdot r_i = 0,0083 \cdot 5 \cdot 7.81 = 0.3227 \ [kN]$

The following pictures compare the results from a hand calculation with the results from the program. As you can see the results fit perfectly together.

Back to our tutorial example we check the results of the necessary beam reinforcement based on the earthquake analysis with accidental eccentricities.

As you see the necessary beam reinforcement was increased from 12.0 cm² to 15.6 cm² in the bottom left column element.

## Tipps and Tricks¶

### Earthquake and Raft Foundations¶

The calculation using the response spectra method is a pure linear elastic calculation. Therefore, the following questions arise in the case of a raft foundation.

1. Are there tensile stresses in the foundation?
2. If yes, how can I recognize this and adjust my model accordingly?

Basically, no node forces and bedding stresses are available as results from a response spectra calculation. This is due to the fact that the individual modes and the directions are superimposed for every single element. Therefore no corresponding forces and moments exist for neighboring elements. However, there are deformation, velocity, and acceleration available as nodal results. These results are always positive. But they will be superimposed with unfavourable sign together with the constant and variable loads. From that results, one can judge about the behaviour of the raft foundation and whether or not a gap occurs. In the case of a gap, it is possible to deactivate the bedding of the raft foundation in partial areas using the SOFiPLUS command “attribute areas”. As a result of the reduced foundation area, a load transfer is simulated, so that there are no lifting forces in the remaining plate. The size of the attribute area must be determined manually and iteratively.

### Earthquake and Piles¶

In case of a pile foundation, modelled with extended piles, DYNA can determine superimposed results. However, the piles are acting for tensile and compressive forces in the same way. Also there are no corresponding forces and moments available for the other piles. Alternatively, the piles can be modeled via spring elements. Here too, the bearing forces of the springs are determined as tensile and compressive forces. In the case of tension springs, these springs could be deactivated by group during the earthquake calculation, thus simulating the failure. For the spring elements it is possible to work with the so-called result sets = RSET. Defining a result set with all springs it is possible to evaluate the maximum spring force of the spring No. 1 including the corresponding spring forces of the remaining springs. The result sets need to be defined in the module SOFiMSHA. A Definition via an SSD task is not yet available. A maximum of 255 springs can be processed in one RSET. You can find an example on RSET in the TEDDY examples of the SOFiMSHA module.

## Literature¶

1. SOFiSTiK AG; DYNA Manual Version 2016
2. Flesch, R.; Baudynamik Praxisgerecht; Band I Berechnungsgrundlagen; Band II Beispiele; Bauverlag Wiesbaden 1993 / 1997
3. Petersen Chr.; Dynamik der Baukonstruktionen, Vieweg Verlag 1996

You will find more references to further literature inside our program manuals

Footnotes

 [1] For the ground acceleration we use g= 10m/s²
 [2] For the ground acceleration we use g= 10m/s²
 [3] For the edge beams only half of the flange overlaps with the slab.

#### Previous page

← Tutorials for Dynamic Analysis

#### Next page

→ Rolling Stock Analysis