T.3 Creating the model using the command file

As an alternatively to the procedures described in the proceeding tutorial, you can also create the same STAAD input file using the STAAD.Pro Editor.

To start a new STAAD input file using the STAAD.Pro Editor, follow the procedure described in Creating a new structure. Then select the Command File tool in the Edit group on the Utilities ribbon tab. The STAAD.Pro Editor window opens with the basic commands for your model entered.

Note: A STAAD input file is a plain text file that uses the .std file extension. Therefore any standard text editor such as Notepad can also be used to create the command file. However, the STAAD.Pro Editor offers the advantage of syntax checking as you type the commands. The STAAD command syntax are highlighted by command, keyword, value, etc.

For this tutorial, delete all the command lines displayed in the editor window and type the lines shown below. While not necessary, this will allow you to learn more about the required and optional command lines for an input file.

STAAD commands are not case sensitive (i.e., they may be typed in upper or lower case letters). By convention, this and most input files use all caps, though.

For most all commands and keywords, the first three letters of a keyword are all that are needed. The rest of the letters of the word are not required, but are useful to present a user-friendly command language in mostly plain English for later reference. By convention, the required letters in a command or keyword are underlined here ("PLANE" = "PLA" = "plane" = "pla").

STAAD SPACE SLAB SUPPORTED ALONG 2 EDGES

Every input has to start with the word STAAD. The word SPACE signifies that the structure is a space frame structure (3-D) and the geometry is defined through X, Y and Z coordinates.

UNIT METER KN

Specifies the unit to be used for data to follow.

JOINT COORDINATES
1 0 0 0 ; 2 2 0 0 ; 3 2 0 2 ; 4 0 0 2 
5 4 0 0 ; 6 4 0 2 ; 7 6 0 0 ; 8 6 0 2 
9 2 0 4 ; 10 0 0 4 ; 11 4 0 4 ; 12 6 0 4

Joint number followed by X, Y and Z coordinates are provided above. Semicolon signs (;) are used as line separators. That enables you to provide multiple sets of data on one line. For example, node 6 has (X, Y, Z) coordinates of (4, 0, 2).

ELEMENT INCIDENCES SHELL
1 1 2 3 4 ; 2 2 5 6 3 ; 3 5 7 8 6 ; 4 4 3 9 10 ; 
5 3 6 11 9 ; 6 6 8 12 11

The incidences of elements are defined above. For example, element 3 is defined as connected between the nodes 5, 7, 8 and 6.

UNIT CM KN
ELEMENT PROPERTY
1 TO 6 THICKNESS 30

The length unit is changed from meter to centimeter. Element properties are then provided by specifying that the elements are 30 cm thick.

UNIT KN  METER
CONSTANTS
E 2.17185e+007 ALL
POISSON 0.17 ALL
DENSITY 23.5616 ALL
ALPHA 1e-005 ALL

Material constants, which are E (modulus of elasticity), Density, Poisson's Ratio and Alpha, are specified following the command CONSTANTS. Prior to this, the input units are changed to Meter and KN.

SUPPORTS
1 2 4 5 7 10 FIXED

Joints 1, 2, 4, 5, 7 and 10 are defined as fixed supported. This will cause all 6 degrees of freedom at these nodes to be restrained.

UNIT KG
LOAD 1 DEAD LOAD

Force units are changed from KN to KG to facilitate the input of loads. Load case 1 is then initiated along with an accompanying title.

SELFWEIGHT Y -1

Load case 1 consists of selfweight of the structure acting in the global Y direction with a factor of -1.0. Since global Y is vertically upward, the factor of -1.0 indicates that this load will act downwards.

LOAD 2 EXTERNAL PRESSURE LOAD

Load case 2 is initiated along with an accompanying title.

ELEMENT LOAD
1 TO 6 PR GY -300

Load 2 is a pressure load on the elements. A uniform pressure of 300Kg/m2 is applied on all the elements. GY indicates that the load is in the global Y direction. The negative sign (-300) indicates that the load acts opposite to the positive direction of global Y.

LOAD 3 TEMPERATURE LOAD

Load case 3 is initiated along with an accompanying title.

TEMPERATURE LOAD
1 TO 6 TEMP 40 30

Load 3 is a temperature load. All the 6 elements are subjected to a in-plane temperature increase of 40 degrees and a temperature variation across the thickness of 30 degrees. This increase is in the same temperature units as the Alpha value specified earlier under CONSTANTS.

LOAD COMB 101 CASE 1 + CASE 2
1 1.0 2 1.0

Load combination 101 is initiated along with an accompanying title. Load cases 1 and 2 are individually factored by a value of 1.0, and the factored values are combined algebraically.

LOAD COMB 102 CASE 1 + CASE 3
1 1.0 3 1.0

Load combination 102 is initiated along with an accompanying title. Load cases 1 and 3 are individually factored by a value of 1.0, and the factored values are combined algebraically.

PERFORM ANALYSIS PRINT STATICS CHECK

The above command instructs the program to proceed with the analysis. A static equilibrium report is also requested with the help of the words PRINT STATICS CHECK.

UNIT METER KN
PRINT ELEMENT STRESS LIST 3

The stresses and unit width moments are requested at the centroid of element 3 in KN and Meter units.

UNIT KG 
METER
PRINT ELEMENT FORCE LIST 6

The forces and moments for all 6 d.o.f at the corner nodes of element 6 are requested in KG and Meter units.

FINISH

This command terminates the STAAD run.

Save the input file and close the editor. The model is opened in the STAAD.Pro interface.