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エディタ.
To start a new STAAD input file using the STAAD.Proエディタ, 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エディタ window opens with the basic commands for your model entered.
STAAD SPACE SLAB SUPPORTED ALONG 2 EDGESEvery 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.
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 4Joint 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 11The 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 30The 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 ALLMaterial 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 FIXEDJoints 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 LOADForce 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 -1Load 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.
ELEMENT LOAD
1 TO 6 PR GY -300Load 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.
TEMPERATURE LOAD
1 TO 6 TEMP 40 30Load 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 1.0Load 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 1.0Load 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 CHECKThe 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 3The stresses and unit width moments are requested at the centroid of element 3 in KN and Meter units.