Buckling Analysis
P-Delta
Click the File menu > New Model command to access the New Model form.
Click the drop-down list to set the units to 
.
Click the Grid Only button 
to access the Quick Grid Lines form. In that form:
Select the Cartesian Tab.
In the Number of Grid Lines area:
Type 1 in the X Direction edit box.
Type 1 in the Y Direction edit box.
Type 2 in the Z Direction edit box.
In the Grid Spacing area, type 12 in the Z Direction edit box.
Click the OK button.
Click the drop-down list in the status bar to change the units to 
.
Click the Define menu > Section Properties > Frame Sections command to access the Frame Properties form.
Click the Add New Property button to access the Add Frame Section Property form. In the Frame Section Property Type drop-down list, select Steel.
Click on the Tube button to access the Box/Tube Section form. In that form:
Type BOX in the Section Name edit box.
Type 20 in the Outside depth (t3) edit box.
Type 20 in the Outside width (t2) edit box.
Type 1 in the Flange thickness (tf) edit box.
Type 1 in the Web thickness (tw) edit box.
Click the + (plus) symbol beside the Material drop-down list to access the Define Materials form. In that form,
Highlight the A992Fy50 material definition in the Materials display area and click the Modify/Show Material button to access the Material Property Data form. In that form:
Ensure that the Units are set to .
Verify that the Modulus of Elasticity is 29000 and Poisson’s Ratio is 0.3.
Click the OK buttons on the Material Property Data and Define Materials forms to close the forms and return to the Box/Tube Section form.
Click the OK buttons on the Box/Tube Section and Frame Properties forms to exit all forms.
Click the drop-down list in the status bar to change the units to .
Click the “X” in the top right-hand corner of the 3-D View window to close that view.
Click the Set XZ View button 
to switch to a XZ view.
Click the Quick Draw Frame/Cable Element button 
to access the Properties of Object form. Verify that the Line Object Type is Straight Frame. Then, highlight (select) BOX from the Section drop-down list.
Click once on the grid line located along the Z axis to draw a frame object.
Click the Set Select Mode button 
to exit Draw mode and enter Select mode.
Click on the point located at the origin (0, 0, 0) to select it.
Click the Assign menu > Joint > Restraints command to access the Joint Restraints form. In that form:
Click the Fixed Base Fast Restraint button 
to set all degrees of freedom (U1, U2, U3, R1, R2 and R3) as restrained.
Click the OK button.
Click the Define menu > Load Pattern command to access the Define Load Patterns form. In that form:
Type LAT in the Load Pattern Name edit box.
Select OTHER from the Type drop-down list.
Click the Add New Load Pattern button.
Type AXIAL in the Load Pattern Name edit box.
Click the Add New Load Pattern button.
Click the OK button.
Click on the frame object to select it.
Click the Assign menu > Frame Loads > Point command to access the Frame Point Loads form. In that form:
Select LAT from the Load Pattern Name drop-down list.
Select X from the Direction drop-down list in the Load Type and Direction area.
Verify that the Relative Distance from End-I option is selected in the Point Loads area.
Type .3333 in the first Distance edit box and type 25 in the first Load edit box.
Type .6667 in the second Distance edit box and type 50 in the second Load edit box.
Click the OK button.
Select the point at the top of the column (0, 0, 12).
Click the Assign menu > Joint Loads > Forces command to access the Joint Forces form. In that form:
Select AXIAL from the Load Pattern Name drop-down list.
Type -1 in the Force Global Z edit box in the Loads area.
Click the OK button.
Click the Show Undeformed Shape button 
to remove the displayed joint force assignments.
Click the Define menu > Load Cases command to access the Define Load Cases form. In that form:
Highlight (select) MODAL in the Load Case Name list and click the Delete Load Case button. Choose Yes when asked if it is ok to delete load case MODAL.
Highlight (select) LAT in the Load Case Name list and click the Modify/Show Load Case button to access the Load Case Data form. In that form:
In the Analysis Type area, select the Nonlinear option.
Select the P-Delta option in the Geometric Nonlinearity Parameters area.
Click the OK buttons on the Load Case Data forms to return to the Define Load Cases form.
In the Define Load Cases form:
Highlight (select) AXIAL in the Load Case Name list and click the Modify/Show Load Case button to access the Load Case Data form. In that form:
Select Buckling from the Load Case Type drop-down list.
In the Stiffness to Use area, select the Stiffness at End of Nonlinear Case option, and verify that LAT is shown in the drop-down list.
Type 2 in the Number of Buckling Modes edit box.
Click the OK buttons on the Load Case Data and Define Load Cases forms to exit all forms.
Click on the frame object to select it.
Click the Assign menu > Frame > Automatic Frame Mesh command to access the Assign Automatic Frame Mesh form. In that form:
Select the Auto Mesh Frame option.
Check the Minimum Number of Segments box and type 4 in the edit box.
Click the OK button.
Click the Run Analysis button 
to access the Set Load Cases to Run form. In that form:
Verify that all load cases are set to Run in the Action list.
Click the Run Now button to run the analysis.
When the analysis is complete, check the messages in the SAP Analysis Monitor window and then click the OK button to close the window.
Click the Display menu > Show Tables command to access the Choose Tables for Display form. In that form:
Click the + (plus) symbol associated with Structure Output item.
Click the + (plus) symbol associated with Other Output Items.
Click the Table: Buckling Factors item to select it.
Click the OK button to display the Buckling Factors table. The product of the Scale Factors shown times the applied axial load gives the critical buckling load. Click the Done button to close the form.