CSI Solution Demonstrates Use of These Features

• Grid lines

• Divide frames

• Frame releases

• Steel Design

Problem A Solution

1. Click the File menu > New Model command to access the New Model form.

2. Click the drop-down list to set the units to .

3. Click the 2D Frames button  to access the 2D Frames form.

   • Select Portal in the 2D Frame Type drop-down list as the template for this model.

   • Type 5 in the Number of Stories edit box.

   • Type 4 in the Number of Bays edit box.

   • Type 13 in the Story Height edit box.

   • Type 25 in the Bay Width edit box.

   • Click the + (plus) symbol beside the down arrow of the Beams or Columns drop-down list to access the Frame Properties form.

   • • Click the Import New Material button to access the Import Frame Section Property form.

     • Select Steel in the Frame Section Property Type drop-down list if it is not already selected.

     • Click the I/Wide Flange button to access the Section Property File form; select the SECTIONS.PRO file and click the Open button to access a database form showing the sections available from the selected database.

     • • On the database form, click the + (plus) symbol preceding the Materials drop-down list to access the Define Materials form. On that form:

       • • Click the Add New Material Quick button to access the Quick Material Definition form. In that form:

         • • Select Steel in the Material Type drop-down list if it is not already selected.

           • Select ASTM A36 from the Specifications drop-down list.

           • Click the OK button on the Quick Material Definition form to return to the Define Materials form.

         • Highlight the A36 definition in the Materials display list and click the Modify/Show button to access the Material Property Data form. In that form:

         • • Verify that the Units are set to .

           • Type 0 in the Weight per Unit Volume edit box.

           • Change the Units to .

           • Ensure that 29500 is the Modulus of Elasticity.

           • Ensure that 0.3 is the Poisson’s Ratio.

           • Type 0 in the Coefficient of Thermal Expansion, A edit box.

           • Verify that 36 is the Minimum Yield Stress, Fy.

           • Verify  that 58 is the Minimum Tensile Stress, Fu.

           • Click the OK button to close the form and return to the Define Materials form.

         • Highlight the 4000Psi definition in the Materials display list and click the Modify/Show Material button to access the Material Property Data form. In that form:

         • • Verify that the Units are set to .

           • Type 4000 in the Modulus of Elasticity edit box.

           • Type .22 in the Poisson’s Ratio edit box

           • Click the Units drop-down list change the units to .

           • Verify 0.15 is displayed in the Weight per Unit Volume edit box.

           • Click the OK button to accept these values and the other values on the form and to close the Material Property Data form and return to the Define Materials form.

         • Click the OK button to close the Define Materials form and return to the database form.

     • On the database form, select the A36 definition from the Materials drop-down list.

     • Scroll down the list of sections, and while holding down the Ctrl key, click on the W10X49, W16X36, and W24X68 sections to select them and access the I/Wide Flange Section form.

     • • Click the OK button on the I/Wide Flange Section form to return to the Frame Sections form.

   • On the Frame Sections form, click the Import New Material button to access the Import Frame Section Property form.

   • • Select Concrete in the Frame Section Property Type drop-down list.

     • Click the Tube button to access the database form showing the sections available from the selected database.  Note that the Section Property File form does not appear because the SECTION.PRO database was opened during the previous section definition, and although the material has been changed for this section definition, the open database contains the selected section type. If the database did not contain the selected section type, the Section Property File form would have displayed:

     • • Verify that the 4000Psi definition is selected in the Materials drop-down list.

       • Scroll down the list of sections and click on the TS6X6X1/4 section to select it.

       • Click the OK button to access the Box/Tube Section form.

       • Click the OK buttons on the Box/Tube Section and Frame Sections forms to close those forms and return to the 2D Frame form.

   • Select the W24X68 section in the Beams drop-down list. Select the W10X49 section in the Columns drop-down list.

   • Click the OK button to close the 2D Frame form and display the model in the program window(s).

4. Click the drop-down list in the status bar to change the units to .

5. Click the Define menu > Section Properties > Area Sections command to access the Area Sections form.

   • On the Area Sections form, select Shell in the Select Section Type to Add drop-down list; then click the Add New Section button to access the Shell Section Data form. In that form:

   • • Type WALL in the Section Name edit box.

     • Verify that the Shell - Thin option is selected in the Type area.

     • In the Thickness area type 8 in both the Membrane and the Bending edit boxes.

     • Click the OK buttons on the Shell Section Data and the Area Sections forms to close all forms.

6. Click the drop-down list in the status bar to change the units to

7. Click the “X” in the top right-hand corner of the 3-D View window to close that view.

8. Click the Set Display Options toolbar button  (or click the View menu > Set Display Options command) to access the Display Options for Active Window form. In that form:

   • Check the Labels box in the Joints area.

   • Check the Labels box in the Frames/Cables/Tendons area.

   • Click the OK button.

9. Select column objects 18, 19, 20, 23, 24 and 25 and beam objects 38, 39, 40, 43, 44 and 45.  Press the delete key on the keyboard to delete those objects.

Note:   Objects can be selected by clicking on each one individually, “windowing” over them, using the Intersecting Line Select Mode, or using the Select menu > Select > Labels command.

10. Click the Define menu > Coordinate Systems/Grids command to access the Coordinate/Grid Systems form.

    • Click on GLOBAL in the Systems list box to highlight it (select it), and then click the Modify/Show System button to access the Define Grid System Data form. In that form:

    • • Check the Glue to Grid Lines box in the right middle of the form.

      • In the X Grid Data area, click in the Ordinate cell for Grid ID x5 (it should read 50 now). Type 53 in the edit box.

      • In the Z Grid Data area, click in the Ordinate cell for Grid ID z1 (it should read 0 now). Type -1 in the edit box.

      • Click the OK button on the Define Grid System Data form and the Coordinate/Grid Systems form.

11. Select beams 41 and 42.

12. Click the Assign menu > Frames > Frame Sections command to access the Frame Properties form.

    • Highlight the W16X36 section in the Properties display list.

    • Click the OK button to assign the section to beams 41 and 42, and to close the Frame Properties form.

13. Click the Get Previous Selection button (or the Select menu > Select > Get Previous Selection command) to reselect beams 41 and 42.

14. Click the Edit menu > Edit Lines > Divide Frames command to access the Divide Selected Frames form.

15.  Fill in the form as shown in the figure  and click the OK button.

16. Verify that the Snap to Points and Grid Intersections button  is depressed.

17. Click the Draw Frame/Cable/Tendon Element button  or select the Draw menu > Draw Frame/Cable/Tendon command to access the Properties of Object form. In that form:

    • Ensure that the Line Object Type is Straight Frame and then click in the Section cell to access a drop-down list. Click on the TS6X6X1/4 section to assign it to the line objects that you will draw.

    • In the Moment Releases drop-down list, click on Pinned.

18. Draw the first brace object as follows:

    • Place the mouse pointer on joint 19. When the text box reading “Grid Point” appears, click the left mouse button once.

    • Move the mouse pointer to joint 31. When the text box reading “Grid Point” appears, click the left mouse button once.

    • Press the Enter key on the keyboard.

19. Click on joint 25 and then joint 31, and press the Enter key to draw the second brace element.

20. Click on joint 20 and then joint 32, and press the Enter key to draw the third brace element.

21. Click on joint 26 and then joint 32, and press the Enter key to draw the fourth and final brace element.

22. Click the Set Select Mode button  to exit the Draw mode and enter the Select mode.

23. Select all of the beams except for the braced frame beams (i.e., select beams 26 through 37 and do not select beams 46 through 49). The Intersecting Line Selection option could be useful for this.

Note:  To use the Intersecting Line Selection option, click the Select Using Intersecting Line button . Then click the left mouse button at the top of one beam bay, and while holding down the left mouse button, drag the mouse to the bottom of the beam bay. A “rubberband line” will appear and all objects that this “rubberband line” passes through will be selected.  Release the left mouse button to make the selection.

24. Click the Assign menu > Frame > Releases/Partial Fixity command to access the Assign Frame Releases form. In that form, check both the Start and the End boxes for Moment 33 (Major) and then click the OK button.

25. Select beam objects 46 and 48.

26. Click the Assign menu > Frame > Releases/Partial Fixity command to access the Assign Frame Releases form. In that form, check the Start box for Moment 33 (Major) and then click the OK button.

27. Select beam objects 47 and 49.

28. Click the Assign menu > Frame > Releases/Partial Fixity command to access the Assign Frame Releases form. In that form, check the End box for Moment 33 (Major) and then click the OK button.

29. Click the Define menu > Load Patterns command to access the Define Load Patterns form. In that form:

    • Type LL in the Load Name edit box.

    • Select Live from the Type drop-down list.

    • Type 0 in the Self Weight Multiplier edit box.

    • Click the Add New Load Pattern button.

    • Type EQ in the Load Name edit box.

    • Select Quake from the Type drop-down list.

    • Select None from the Auto Lateral Load drop-down list.

    • Click the Add New Load Pattern button.

    • Click the OK button.

30. Click the Define menu > Load Combinations command to access the Define Load Combinations form. In that form:

    • Click the Add New Combo button to access the Load Combination Data form. In that form:

    • • Type ALL in the Load Combination Name edit box.

      • Select Linear Add from the Load Combination Type drop-down list if it is not already selected.

      • If not already set, select the DEAD load pattern in the Load Case Name drop-down list and type 1 in the Scale Factor edit box.

      • Click the Add button.

      • Select the LL load pattern in the Load Case Name drop-down list.

      • Click the Add button.

      • Select the EQ load pattern in the Load Case Name drop-down list.

      • Click the Add button.

      • Click the OK button on the Load Combination Data form and the Define Load Combinations form.

31. Select beams 26 through 37.

32. Click the Assign menu > Frame Loads > Point command to access the Frame Point Loads form. In that form:

    • Select DEAD from the Load Pattern Name drop-down list.

    • In the Load Type and Direction area, make sure that Forces is selected and that Gravity (-Z) shows in the Direction drop-down list.

    • In the Point Loads area type .5 in the first Distance edit box and type 10 in the first Load edit box.

    • Click the OK button.

33. Click the Get Previous Selection button  (or the Select menu > Get Previous Selection command).

34. Click the Assign menu > Frame Loads > Distributed command to access the Frame Distributed Loads form. In that form:

    • Select DEAD from the Load Pattern Name drop-down list.

    • In the Load Type and Direction area, make sure that Forces is selected and that Gravity (-Z) shows in the Direction drop-down list.

    • Type 1.2 in the Uniform Load area Load edit box.

    • Click the OK button.

35. Click the Get Previous Selection button  (or the Select menu > Get Previous Selection command).

36. Click the Assign menu > Frame Loads > Point command to access the Frame Point Loads form. In that form:

    • Select LL from the Load Pattern Name drop-down list.

    • In the Point Loads area type 5 in the first Load edit box

    • Click the OK button.

37. Click the Get Previous Selection button  (or click the Select menu > Get Previous Selection command).

38. Click the Assign menu > Frame Loads > Distributed command to access the Frame Distributed Loads form. In that form:

    • Select LL from the Load Pattern Name drop-down list.

    • In the Load Type and Direction area, make sure that Forces is selected and that Gravity (-Z) shows in the Direction drop-down list.

    • Type .8 in the Uniform Load area Load edit box.

    • Click the OK button.

39. Select beams 46 through 49.

40. Click the Assign menu > Frame Loads > Distributed command to access the Frame Distributed Loads form. In that form:

    • Select DEAD from the Load Pattern Name drop-down list.

    • Type 1.2 in the Uniform Load area Load edit box.

    • Click the OK button.

41. Click the Get Previous Selection button   (or click the Select menu > Get Previous Selection command).

42. Click the Assign menu > Frame Loads > Distributed command to access the Frame Distributed Loads form. In that form:

    • Select LL from the Load Pattern Name drop-down list.

    • Type .8 in the Uniform Load area Load edit box.

    • Click the OK button.

43. Select joints 31 and 32.

44. Click the Assign menu > Joint Loads > Forces command to access the Joint Forces form. In that form:

    • Select DEAD from the Load Pattern Name drop-down list.

    • Type -10 in the Force Global Z edit box in the Loads area.

    • Click the OK button.

45. Click the Get Previous Selection button   (or the Select menu > Get Previous Selection command).

46. Click the Assign menu > Joint Loads > Forces command to access the Joint Forces form. In that form:

    • Select LL from the Load Pattern Name drop-down list.

    • Type -5 in the Force Global Z edit box in the Loads area.

    • Click the OK button.

47. Select joints 2, 3, 4, 5 and 6 by “windowing.”

48. Click the Assign menu > Joint Loads > Forces command to access the Joint Forces form. In that form:

    • Select EQ from the Load Pattern Name drop-down list.

    • Type 10 in the Force Global X edit box in the Loads area.

    • Type 0 in the Force Global Z edit box in the Loads area.

    • Click the OK button.

49. Select joints 3, 4, 5 and 6 (not 2) by “windowing.”

50. Click the Assign menu > Joint Loads > Forces command to access the Joint Forces form. In that form:

    • Verify Add to Existing Loads is selected in the Options area.

    • Click the OK button.

51. Select joints 4, 5 and 6 (not 2 and 3) by “windowing.”

52. Click the Assign menu > Joint Loads > Forces command to access the Joint Forces form. In that form:

    • Verify Add to Existing Loads is selected in the Options area.

    • Click the OK button.

53. Select joints 5 and 6 (not 2, 3 and 4).

54. Click the Assign menu > Joint Loads > Forces command to access the Joint Forces form. In that form:

    • Verify Add to Existing Loads is selected in the Options area.

    • Click the OK button.

55. Select joint 6 (not 2, 3, 4 and 5).

56. Click the Assign menu > Joint Loads > Forces command to access the Joint Forces form. In that form:

    • Verify Add to Existing Loads is selected in the Options area.

    • Click the OK button.

57. Click the Set Display Options button  (or select the View menu > Set Display Options command) to access the Display Options for Active Window form. In that form:

    • Uncheck the Labels box in the Joints area.

    • Uncheck the Labels box in the Frames/Cables/Tendon area.

    • Click the OK button.

58. Click the Quick Draw Area Element button  to access the Properties of Object form. Verify that  WALL is selected in the Section drop-down list.

59. Click the mouse pointer once in the areas labeled A, B, C, D and E in the figure below to draw the area objects.

60. Click the Set Select Mode button to exit Draw mode and enter Select mode.

61. Select the five area objects just entered by clicking on them.

62. Click the Assign menu > Area > Automatic Area Mesh command to access the Assign Automatic Area Mesh form.

63. Fill out that form as shown in the figure to mesh each area object into twelve elements (4 by 3) and click the OK button.

64. Click the Set Display Options button  (or select the View menu > Set Display Options menu) to access the Display Options for Active Window form. In that form:

    • Check the Not in View box in the Joints area.

    • Check the Sections box in the Frames/Cables/Tendon area.

    • Check the Not in View box in the Areas area.

    • Click the OK button.

65. Select all of the W24X68 beam sections (12 total).

66. Click the Design menu > Steel Frame Design > View/Revise Overwrites command to access the Steel Frame Design Overwrites form. In that form:

    • Select the Unbraced Length Ratio (Minor, LTB) box and type .3333 in the associated edit box.

    • Click the OK button.

67. Click the Clear Selection button  (or click the Select menu > Clear Selection command).

68. Select all of the W16X36 beam sections (4 total). This can be accomplished using the Select menu > Select > Properties > Frame Sections command, which accesses the Select Section form. Click on the W16X36 section in the display list and click the OK button. The beams are selected in the model.

69. Click the Design menu > Steel Frame Design > View/Revise Overwrites command to access the Steel Frame Design Overwrites form. In that form:

    • Select the Unbraced Length Ratio (Minor, LTB) box and type .5 in the associated edit box.

    • Click the OK button.

70. Click the Clear Selection button  (or click the Select menu > Clear Selection command).

71. Click the Set Display Options button  (or select the View menu > Set Display Options command) to access the Display Options for Active Window form. In that form:

    • Uncheck the Not in View box in the Joints area.

    • Check the Restraints box in the Joints area.

    • Uncheck the Sections box in the Frames/Cables/Tendon area.

    • Uncheck the Not in View box in the Areas area.

    • Click the OK button.

72. Click the Design menu  > Steel Frame Design > View/Revise Preferences command to access the Steel Frame Design Preferences form. In that form:

    • Select AISC-ASD89 from the Design Code drop-down list.

    • Click the OK button.

73. Click the Analyze menu > Set Analysis Options command to access the Analysis Options form. In that form, click the Plane Frame XZ Plane button to set the available degrees of freedom and click the OK button.

74. Click the Run Analysis button  to access the Set Load Cases to Run form. In that form:

    • Click on Modal in the Case Name list to highlight it.

    • Click the Run/Do Not Run Case button.

    • Click the Run Now button.

75. When the analysis is complete, check the messages in the Analysis window (there should be no warnings or errors) and then click the OK button to close the Analysis window.

76. Click the Display menu > Show Forces/Stresses > Joints command to access the Joint Reaction Forces form. In that form:

    • Select ALL from the Case/Combo Name drop-down list.

    • Click the OK button. The reactions are displayed on the screen. If the text is too small to read, zoom in, or change the minimum font size as described in the following Note.

Note:   To change the minimum font size, click the Options menu > Dimensions/Tolerances command.  In the Minimum Graphic Font Size edit box, input a new size, for example 5 or 6 points. Click the OK button. 

77. Click the Design menu > Steel Frame Design > Start Design/Check of Structure command to run the design check of the steel frame objects.

78. When the design check completes, a color map of the stress ratios is displayed.