# T.1 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.

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 PLANE PORTAL FRAME``

Every STAAD input file has to begin with the word STAAD. The word PLANE signifies that the structure is a plane frame (in the XY plane). The remainder of this line is the title of the problem, which is optional.

Note: If a line is typed with an asterisk in the first column, it signifies that the line is a comment line and should not be executed. For example, one could have put the optional title above on a separate line as follows:

``* PORTAL FRAME``
``UNIT FEET KIP``

Specify the force and length units for the commands to follow.

``````JOINT COORDINATES
1 0. 0. ; 2 0. 15. ; 3 20. 15. ; 4 20. 0.``````

Joint numbers and their corresponding global X and Y coordinates are provided above. For example, 3 20 15. indicates that node 3 has an X coordinate of 20 ft and a Y coordinate of 15 ft. Note that the reason for not providing the Z coordinate is because the structure is a plane frame. If this were a space frame, the Z coordinate would also be required.

Semicolons (;) are used as line separators. In other words, data which is normally put on multiple lines can be put on one line by separating them with a semicolon.

``````MEMBER INCIDENCE
1 1 2 ; 2 2 3 ; 3 3 4``````

The members are defined by the joints to which they are connected.

``````MEMBER PROPERTY AMERICAN
1 3 TABLE ST W12X35
2 TABLE ST W14X34``````

Members 1 and 3 are assigned a W12X35 section from the built-in AMERICAN steel table. Member 2 has been assigned a W14X34. The word ST stands for standard single section. Refer to subsections 1 through 5 of TR.20 Member Property Specification for details on the convention for assigning member property names.

``````UNIT INCHES
DEFINE MATERIAL START
ISOTROPIC STEEL
E 29000
POISSON 0.3
DENSITY 283e-006
ALPHA 6e-006
DAMP 0.03
TYPE STEEL
STRENGTH FY 36 FU 58 RY 1.5 RT 1.2
END DEFINE MATERIAL``````

And to use this material definition for all members, add the following:

``````CONSTANTS
MATERIAL STEEL ALL``````

The length unit is changed from FEET to INCHES to use familiar units for most of the material definition. For this example, you use a set of built-in values for steel, so the units are only shown for convenience here. In the user interface, units were not changed until the following commands were generated. See TR.26.1 Define Material for more information.

``````MEMBER OFFSET
2 START 6.0 0. 0.
2 END -6.0 0. 0.``````

The beam member is physically connected to the 2 columns at the face of the column, and not at the column centerline. This creates a rigid zone, about half the depth of the columns, at the 2 ends of the beam 2. This rigid zone is taken advantage of using member offsets (It is you choice whether or not you wish to use these). So, the above commands define that member 2 is eccentrically connected or OFFSET at its START joint by 6 inches in the global X direction, 0.0 and 0.0 in Y and Z directions. The same member is offset by negative 6.0 inches at its END joint. See TR.25 Member Offset Specification for more information.

``PRINT MEMBER INFORMATION ALL``

The information that is printed by this command includes start and end joint numbers (incidence), member length, beta angle and member end releases.

``````SUPPORTS
1 FIXED ; 4 PINNED``````

A fixed support is located at joint 1 and a pinned support (fixed for translations, released for rotations) at joint 4. More information on the support specification is available in TR.27 Support Specifications.

``UNIT FT``

The length unit is changed to FEET to facilitate input of loads.

``````LOADING 1 DEAD + LIVE
2 UNI GY -2.5``````

The above commands identify a loading condition. DEAD + LIVE is an optional title to identify this load case. A Uniformly distributed MEMBER LOAD of 2.5 kips/ft is acting on member 2 in the negative global Y direction. Member Load specification is explained in TR.32 Loading Specifications.

``````LOADING 2 WIND FROM LEFT
2 FX 10.``````

The above commands identify a second load case. This load is a JOINT LOAD. A 10 kip force is acting at joint 2 in the global X direction.

``````LOAD COMBINATION 3 75 PERCENT OF (DL+LL+WL)
1 0.75 2 0.75``````

This command identifies a combination load with an optional title. The second line provides the components of the load combination case - primary load cases and the factors by which they should be individually multiplied.

``PERFORM ANALYSIS PRINT STATICS CHECK``

This command instructs the program to proceed with the analysis and produce a report of static equilibrium checks. TR.37 Analysis Specification offers information on the various analysis options available.

``````PRINT MEMBER FORCES ALL
PRINT SUPPORT REACTION LIST 1 4``````

The above print commands are self-explanatory. The member forces are in the member local axes while support reactions are in the global axes.

``````LOAD LIST 1 3
PARAMETER 1
CODE AISC UNIFIED 2010
FYLD 7200 ALL
TRACK 2.0 MEMB 2 3
UNB 10.0 MEMB 2 3
UNT 10.0 MEMB 2 3
SELECT MEMBER 2 3``````

The above sequence of commands is used to initiate the steel design process. The command PARAMETER is followed by the various steel design parameters. Parameters are specified typically when their values differ from the built-in program defaults. Specifications of the AISC Unified Code LRFD specification are to be followed. A parameter list for the AISC code is available in D1.A.6 Design Parameters. Member numbers 2 and 3 have 10 ft unsupported length for the top and bottom flange (UNT and UNB).

UNT and UNB are used to compute the allowable compressive stress in bending. The yield strength, FYLD, of steel is specified as 7,200 ksf (50 ksi) since it is different from the default value of 36 ksi and it is assigned to ALL members. The TRACK parameter controls the level of description of the output, 2.0 being the most detailed. The LOAD LIST command lists the load cases (1 and 3) to be used in the design. The SELECT MEMBER command asks the program to evaluate the most economical section for members 2 and 3 in the context of the above analysis.

``PERFORM ANALYSIS``

When the analysis and design engine executes the member selection operation specified in the member selection , a new set of properties will end up being assigned to those members. This has the effect of changing the stiffness distribution for the entire structure. Since the structure is statically indeterminate, it is best practice to re-analyze it to determine the accurate nodal displacements, member forces, etc. which reflect this new stiffness distribution. The above command instructs the program to do another cycle of analysis.

``````PARAMETER 2
TRACK 0 ALL``````

The TRACK parameter is specified again in a new PARAMETER set. It controls the level of information produced in the steel design output. This time, the value of 0 is used to provide a pass or fail status for each member.

``CHECK CODE ALL``

The analysis operation carried out earlier will create a new set of member forces. These forces will very likely be different from those which were used in the member selection operation. Consequently, you should verify that the structure is safely able — from the standpoint of the design code requirements — to carry these new forces. A code checking operation, which uses the up-to-date cross sections of the members, and the latest member forces, will provide a status report on this issue.

``FINISH``

A STAAD run is terminated using the FINISH command.

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

This concludes the session on generating the model as a command file using the built-in editor. If you wish to perform the analysis and design, you may proceed to the next section of this manual. The post-processing facilities are explained in Post Processing.

CAUTION: Remember that without successfully completing the analysis and design, the post-processing facilities will not be accessible.