STAAD.Pro Help

TR.42 Print Specifications

This command is used to direct the program to print various modeling information and analysis results. STAAD.Pro offers a number of versatile print commands that can be used to customize the output.

General Format

Data Related Print Commands 

PRINT { PROBLEM STATISTICS | JOINT COORDINATES | MEMBER PROPERTIES | ELEMENT INFORMATION (SOLID) | MATERIAL PROPERTIES | SUPPORT INFORMATION | ALL } { (ALL) | LIST item/joint/member-list }

Print Location of CG 

PRINT CG (_group_name)

Print Analysis Results 

PRINT { (JOINT) DISPLACEMENTS | MEMBER FORCES (GLOBAL) | ANALYSIS RESULTS| MEMBER SECTION FORCES | MEMBER STRESSES | ELEMENT (JOINT) STRESSES (AT f1 f2) | ELEMENT FORCES | ELEMENT (JOINT) STRESSES SOLID | MODE SHAPES } list-spec
list-spec = { (ALL) | LIST joint/member/elements-list }

Print Support Reactions 

PRINT SUPPORT REACTIONS

Print Story Drifts or Stiffness 

PRINT STORY DRIFT (f3)
PRINT STORY STIFFNESS

Print Location of Center of Rigity at each Floor 

PRINT DIAPHRAGM CR

Print the deflected (sag) shape of a cable after an advanced cable analysis: 

PRINT CABLE SAG

Description

The list of items is not applicable for PRINT ANALYSIS RESULTS and PRINT MODE SHAPES commands.

The PRINT JOINT COORDINATES command prints all interpreted coordinates of joints.

The PRINT MEMBER INFORMATION command prints all member information, including member length, member incidences, beta angles, whether or not a member is a truss member and the member release conditions at start and end of the member (1 = released, 0 = not released).

The PRINT ELEMENT INFORMATION command prints all incident joints, element thicknesses, and Poisson ratios for Plate/Shell elements. The PRINT ELEMENT INFORMATION SOLID command prints similar information for Solid elements.

The PRINT MEMBER PROPERTIES command prints all member properties including cross sectional area, moments of inertia, and section moduli in both axes. Units for the properties are always INCH or CM (depending on FPS or METRIC) regardless of the unit specified in UNIT command.

The following designation is used for member property names:

AX
Cross section area
AY
Area used to adjust shear/bending stiffness in local Y axis to account for pure shear in addition to the classical bending stiffness
AZ
Area used to adjust shear/bending stiffness in local Z axis to account for pure shear in addition to the classical bending stiffness.
IZ
Moment of Inertia about the local Z-axis
IY
Moment of Inertia about the local Y-axis
IX
Torsional constant
SY
Smallest section modulus about the local Y-axis
SZ
Smallest section modulus about the local Z-axis

The PRINT MATERIAL PROPERTIES command prints all material properties for the members, including E (modulus of elasticity), G (shear modulus), weight density and coefficient of thermal expansion (alpha) for frame members. This command is available for members only. G may be listed as zero if command is before load cases and Poisson ratio was entered but G was not entered.  

The PRINT SUPPORT INFORMATION command prints all support information regarding their fixity, releases and spring constant values, if any.  The LIST option is not available for this command.

The PRINT ALL command is equivalent to last five print commands combined. This command prints joint coordinates, member information, member properties, material properties and support information, in that order.

The PRINT CG command prints out the coordinates of the center of gravity and the total weight of the structure or of a single group of member/elements. If the CG of a portion of the structure is desired, the members and elements of that portion must be assigned using a group name (see TR.16 Entities as Single Objects for details on using group-names). Only the selfweight of the structure is used to calculate the C.G. User defined joint loads, member loads etc. are not considered in the calculation of C.G. 

The PRINT (JOINT) DISPLACEMENTS command prints joint displacements in a tabulated form. The displacements for all six directions will be printed for all specified load cases. The length unit for the displacements is always INCH or CM (depending on FPS or METRIC unit) regardless of the unit specified in UNIT command.

The PRINT (MEMBER) FORCES command prints member forces (i.e., Axial force (AXIAL), Shear force in local Y and Z axes (SHEAR-Y and SHEAR-Z), Torsional Moment (TORSION), Moments about local Y and Z axes (MOM-Y and MOM-Z)) in a tabulated form for the listed members, for all specified load cases. The GLOBAL option will output forces in the global coordinate system rather than the member local coordinate system for each member.

The PRINT SUPPORT REACTIONS command prints global support reactions in a tabulated form, by support, for all specified load cases. Use LIST option for selected joints. 

The PRINT ANALYSIS RESULTS command is equivalent to the above three commands combined. With this command, the joint displacements, support reactions and member forces, in that order, are printed.

The PRINT (MEMBER) SECTION FORCES command prints axial force, shear forces, & bending moments at the intermediate sections specified with a previously input SECTION command. The printing is done in a tabulated form for all specified cases for the first requested member, then for the next member, etc.

Note: An asterisk following a critical load case number within PRINT JOINT DISPLACEMENT, PRINT MEMBER FORCES, PRINT SECTION FORCES,PRINT MEMBER STRESS, or PRINT SUPPORT REACTION outputs indicates that this load case is a generated load combination. See TR.35 Load Combination Specification for additional information.

The PRINT (MEMBER) STRESSES command tabulates member stresses at the start joint, end joint and all specified intermediate sections. These stresses include axial (i.e., axial force over the area), bending-y (i.e., moment-y over section modulus in local y-axis), bending-z (i.e., moment-z over section modulus in local z-axis), shear stresses in both local y and z directions (shear flow, q, over the shear area), and combined (absolute combination of axial, bending-y and bending-z) stresses.

  • For PRISMATIC sections, if AY and/or AZ is not provided, the full cross-sectional area (AX) will be used.
  • For TAPERED sections, the values of AY and AZ are those for the location where the stress is printed.  Hence at the location 0.0, the AY and AZ are based on the dimensions of the member at the start node.

The PRINT ELEMENT STRESSES command must be used to print plate stresses (SX, SY, SXY, SQX, SQY), moments per unit width (MX, MY, MXY) and principal stresses (SMAX, SMIN, TMAX) for plate/shell elements. Typically, the stresses and moments per unit width at the centroid will be printed. The Von Mises stresses (VONT, VONB) as well as the angle (ANGLE) defining the orientation of the principal planes are also printed.

The variables that appear in the output are the following. Refer to G.5.1 Plate and Shell Elements for more information regarding these variables.

SQX
Shear stress on the local X face in the Z direction
SQY
Shear stress on the local Y face in the Z direction
MX
Moment per unit width about the local X face
MY
Moment per unit width about the local Y face
MXY
Torsional Moment per unit width in the local X-Y plane
SX
Axial stress in the local X direction
SY
Axial stress in the local Y direction
SXY
Shear stress in the local XY plane
VONT
Von Mises stress on the top surface of the element
VONB
Von Mises stress on the bottom surface of the element
TrescaT
Tresca stress on the top surface of the element
TrescaB
Tresca stress on the bottom surface of the element
SMAX
Maximum in-plane Principal stress
SMIN
Minimum in-plane Principal stress
TMAX
Maximum in-plane Shear stress
ANGLE
Angle which determines direction of maximum principal stress with respect to local X axis
Note: If the JOINT option is used, forces and moments at the nodal points are also printed out in addition to the centroid of the element.

The AT option may be used to print element forces at any specified point within the element. The AT option must be accompanied by f1 and f2. f1 and f2 are local X and Y coordinates (in current units) of the point where the stresses and moments are required. For detailed description of the local coordinate system of the elements, refer to G.5 Finite Element Information.

The PRINT ELEMENT FORCES command enables printing of plate "corner forces" [ Fp = Kp • Dp ] in global axis directions.

The PRINT ELEMENT (JOINT) STRESS SOLID command enables printing of stresses at the center of the SOLID elements.  The variables that appear in the output are the following.

Normal Stresses
SXX, SYY and SZZ
Shear Stresses
SXY, SYZ and SZX
Principal Stresses
S1, S2 and S3.
Von Mises Stresses
SE
Direction cosines
Six direction cosines are printed following the expression DC, corresponding to the first two principal stress directions.
Note: The JOINT option will print out the stresses at the nodes of the solid elements.

The PRINT MODE SHAPES command prints the relative joint motions of each of the modes that were calculated. The maximum motion is arbitrary and has no significance. Dynamic analysis will scale and combine the mode shapes to achieve the final dynamic results.   

Example

PERFORM ANALYSIS
PRINT ELEMENT JOINT STRESS
PRINT ELEMENT STRESS AT 0.5 0.5 LIST 1 TO 10
PRINT SUPPORT REACTIONS
PRINT JOINT DISPLACEMENTS LIST 1 TO 50
PRINT MEMBER FORCES LIST 101 TO 124

Example

Printing the Center of Gravity (CG) 

PRINT CG
PRINT CG _RAFTERBEAMS
PRINT CG _RIDGEBEAMS

Notes

  1. The output generated by these commands is based on the current unit system. The user may wish to verify the current unit system and change it if necessary.

  2. Results may be printed for all joints/members/elements or based on a specified list.

Printing the Story Drift and Stiffness

The PRINT STORY DRIFT command may be used to obtain a print-out of the average lateral displacement of all joints at each horizontal level along the height of the structure.

The procedure used in STAAD.Pro for calculating story drift is independent of any code. For example, the story drift determination as explained in section 12.8.6 of the ASCE 7-05 code is not implemented in STAAD.Pro.

The method implemented in STAAD.Pro involves:

  1. Find all the distinct Y coordinates in the model. Those are what STAAD.Pro calls as stories.

  2. For each of those distinct stories, find all the nodes at that story elevation.

  3. For each story, find the average displacement along the horizontal directions (X and Z) by adding up corresponding displacement for all the nodes at that story, and dividing by the number of nodes for that story. Thus, even if there is only a single node representing a story, a drift is calculated for that story too.

In STAAD.Pro if PRINT STORY DRIFT command is issued, the program prints the average of horizontal displacements of all the joints present at the particular floor level.

However, to check inter-story drift, the following commands needs to be issued after the PERFORM ANALYSIS command. 

LOAD LIST i1
PRINT STORY DRIFT f3

Where:

  • i1 = the primary load number for which inter-story drift check is required
  • f3 = The allowable drift factor, as per the code provision

The program will calculate the relative horizontal displacement between two adjacent floors. This calculated value is checked against the allowable limit. The result is reported as either "PASS" or "FAIL" in the output.

Note: There is only one exception to this format. For IS 1893: 2002 static seismic load case, even if this factor is not provided the program internally checks if the loading is IS 1893 static seismic loading or not. If yes, it automatically calculates the inter-story drift and checks against the code provisions.

For dynamic IS 1893: 2002 response spectrum analysis the above format for inter-story drift check does not hold true. The reason is that in response spectrum analysis the joint displacements represents the maximum magnitude of the response quantity that is likely to occur during seismic loading. Any response quantity like story drift should be calculated from actual displacements of each mode considered during analysis. The inter-story drift from each mode is combined using modal combination to get the maximum magnitude of this response quantity. In order to compute story drift for IS 1893 response spectrum the load case command format described in TR.32.10.1.7 Response Spectrum Specification per IS: 1893 (Part 1)-2002 must be used..

The PRINT STORY STIFFNESS command may be used to include the calculated lateral stiffness of each story used in determining the drift. In STAAD.Pro lateral stiffness is calculated only when the floor is modeled as rigid floor diaphragm since it functions as transferring story shears and torsional moments to lateral force-resisting members during earthquake.

Printing the Center of Rigidity & Center of Mass

The PRINT DIAPHRAGM CR command may be used to obtain a print-out of the center of rigidity and center of mass at each rigid diaphragm in the model. The lateral force at each floor, as generated by earthquake and wind loading, acts at the center of rigidity of each floor which is modeled as rigid floor diaphragm. The center of mass of each floor is defined as the mean location of the mass system of each floor. The mass of the floor is assumed to be concentrated at this point when the floor is modeled as rigid diaphragm. The distance between these two is the lever arm for the natural torsion moment for seismic loads when that option is used.

Parent topic: Technical Reference of STAAD Commands
Related conceptsRelated tasksRelated reference