Subjects Covered

• Composite beam structures
• FE webs; 3D structures
• Virtual members
• Member eccentricities
• Joint editing

Outline

This access bridge is constructed with two steel plate girders supported on “H” piles acting compositely with a concrete slab. The top flange of the beam has an arched profile and it is deeper in the centre than at the ends.

The slab, diaphragm and upstand are created with grade C32/40 concrete and the girder with grade 355 structural steel.

The structure is modelled using a 3D shell finite element slab (curved in elevation) with a steel composite beam inserted as an FE web beam to explicitly model the web as finite elements and the flanges as beam elements. Upstands are added as edge beam members with the appropriate vertical offset and the diaphragm is represented with finite elements.

The beam, a 30m span, is assumed to be continuous at its ends as there will be some hogging at this location and this will affect the effective breadth of concrete flange. The adjacent spans (the piles) are assumed to be 4m long and fixed into rock at the remote end.

The girder has uniform thickness of web and flanges throughout (28mm & 50mm respectively) and the flanges are 500mm wide. The overall depth is set to 1000mm deep but with a sagging profile such that the overall depth at the ends is 500mm. This is done with 20 straight segments, as the curved profile is limited to hogging shapes. The profile points are not exactly on a circular curve but are close to it.

The slab in the beam representation is 2m wide and 0.2m thick, but is offset by 0.5m.

An edge upstand 200mm wide and 250mm deep is added above each edge of the slab and is assumed to be structural and cast with the slab.

Mid Span Section

Profile of Top Of Beam
0.00	0.00
1.50	0.19
3.00	0.36
4.50	0.51
6.00	0.64
7.50	0.75
9.00	0.84
10.50	0.91
12.00	0.96
13.50	1.00
15.00	1.00
16.50	1.00
18.00	0.96
19.50	0.91
21.00	0.84
22.50	0.75
24.00	0.64
25.50	0.51
27.00	0.36
28.50	0.19
30.00	0.00

The carriageway on the bridge is a single lane of 3.8m, centred on the deck, with no footway or verges.

Procedure

The general procedure is as follows:

• Create a Beam for a composite girder and add tiles etc.

  • Define the materials needed
  • Define a composite design beams representing the north girder
  • Save the beam for subsequent use in a structural project.

• Create a structural project and add title etc.

• Define a design beam in the project using the save file and embed the data (which will add material properties to the project).

• Create a 2D sub-model consisting of a flat 2d finite element slab and the edge upstand beams.

• Change the 2D sub-model to 3D and adjust vertical coordinates to give a vertically curved slab.

• Create design section in the project to represent the upstand and the piles.

• Assign the composite girders to the structure as “FE Web” members and the edge section to the edge beam elements.

• Define two 2D sub-models containing the piles and diaphragms and assign properties and supports.

• Define dead load and SDL load cases and compilations.

• Live load optimisation for one point on the south main girder.

• Analyse the structure/load cases.

• Transfer the results to the design beam load effect tables.

• Perform one or two design checks.

  Beam Definition

Only one girder needs to be defined (the north one) as it can be mirrored for the south girder.

1. Start the program and create a new beam using the main menu File | New | Create from template selecting “EU Steel Composite” from the list.

2. Use the main menu File | Titles... to set a title for the beam as “Composite banana beam” with a sub title of “Example 10.2”, a Job Number of “10.2” and add your initials in the Calculations by: field before closing with ✓ OK.

3. In the Materials navigation window delete the concrete material C40/50 and the prestress material Grade 1637 by selecting them, one by one, and using the navigation toolbar button , which will leave three materials.

4. Open the structural steel S355/355 material and change the Yield Strength to “345” to make it S355/345 before closing the form with ✓ OK.

5. Define a second structural steel material S355/335.

6. In the Design Beam navigation window select the item Beam Definition to open the Define Composite Beam form.

7. Set the MAIN SPAN to be “Continuous-internal span” with a span of 30m and the SIDE SPANS as “End spans” with spans of 4.0m (accept the warning message about spans being outside expected range).

8. Set the Cross section to “uniform” and the Location as “Inner beam”.

9. In the Define field select “Section” to open the Composite Beam Section Definition form.

10. Create a “Hybrid Girder - I” component with “500mm” wide flanges and a “1000mm” depth overall. The thickness of flange and web are “50mm” and “28mm” respectively.

11. Close the Component form using the ✓ OK button.

12. Click in the Property field for this component which allows different grades of steel to be assigned to each plate component.

13. Assign S355/345 to the web and S355/335 to both flanges.

    

14. Create a second component as a “Concrete Slab” setting the slab Width to be 2000mm and the Depth to be 200mm.

15. Close the component form using the ✓ OK button.

16. In the Slab Details set the Y offset to be 0.5m.

17. Now add a third component as “Concrete Edge” and create 5 coordinate points by using the “+” button at the bottom of the form and entering the data as shown below:

    

18. Close the User Defined Edge Detail form with the ✓ OK button and ensure the material properties are assigned correctly (grade C32/40 concrete) and that the edge detail is structural and it is cast with the slab.

    

19. Close the Section Definition form, then note and click Yes on the confirm form.

20. Open the Define soffit profile form using the appropriate option in the Define field.

21. Enter the profile points into the table as shown below:

Proportion of span	Offset (mm)
0.0	500
0.1	320
0.2	180
0.3	80
0.4	20
0.5	0
0.6	20
0.7	80
0.8	180
0.9	320
1.0	500

The general beam has now been defined – lateral restraints, web stiffeners and shear connecters may be added in the design stage.

22. Close all the open forms (using the ✓ OK button) and save the file as “My EU Example 10_2 banana_beam.sam” using the File | Save as... menu option.

    Project Setup Including Design Beam and Sections

    The first steps in creating the structural model can now be taken by defining the design Sections to be used and setting up the flat slab 30m long by 4m wide. There will be 20 equally spaced elements longitudinally and 6 elements transversely, with the edge element 0.5m and the internal element 0.75m.

23. Begin a new project using the main menu File | New | Create From Template... and selecting “EU Project” from the options.

24. In the Titles form add a Project Title of “Composite Banana Bridge” with a subtitle “EU Example 10.2” and Job Number: “10.2”.

25. Add your initials in the Calculations by: field.

26. In the Materials navigation window delete all the materials using the Clear All task as the required materials will be defined when the beam file is imported.

27. In the Design Beam navigation window toolbar click on to add an “Existing Design Beam” and select the beam file “EU Example 10_2 Banana_beam.sam”. Then click the icon on the toolbar to embed the beam (also creating the project materials).

28. In the Design Sections navigation window click on the button, select New Section | Parametric Shape and add a rectangular parametric shape, 200mm wide by 250mm deep.

29. Set the Hook Point Reference to 1 with coordinates Y “0” and Z “100” (to give it the correct elevation with respect to the slab centre).

30. Set the property to the C32/40 concrete material before closing the form with ✓ OK.

31. Rename this Design Section to “Edge Upstand” using the right mouse button in the navigation window.

    It is also necessary to define a Design Section for the “H” shaped piles, again using a parametric shape.

32. Click on the toolbar button to select New Section | Parametric Shape....

33. Set Shape Reference to H and enter a width and height of 450mm.

34. Enter a thickness of 28mm for both horizontal and vertical and change Property to “S355/345”.

35. The Hook Point Reference should be set to “0” with Y and Z Coordinates of “0” and “0”.

36. Close the form with ✓ OK and then rename the section in the navigation window to “H Piles”.

    Creating the Flat Slab

37. In the main menu, select Data | Structure Type | Refined Analysis to ensure this is the current structure type.

38. In the Structure Definition navigation window toolbar click on to create a new 2D sub-model (GCS, z=0.0) to the structure.

39. Add a new mesh to this sub-model and create a Finite Element mesh using a Mesh Type of “Orthogonal to span” and pick mode “by point” (remember to set the Member Type: radio button to “Finite Elements”).

40. Set the Snap mode to “Grid” in the graphics window tool bar and click on the appropriate grid points in the graphic window to define the boundary of the slab (30m x 4m). The display of the coordinates in the top right hand corner can be used for guidance.

41. Set the number of elements transversely to 6 and longitudinally to 20 then change the “Equal Size” option for the transverse elements to “Set Size”.

42. In the Set Transverse Size form that should now be visible set the spacing factors as shown below for the elements and then close this form with the ✓ OK button.

43. Change the Name: of the mesh to “Slab” and close the meshing form in the usual way. A warning message about aspect ratio size may be displayed which will be acceptable so click on Continue.

    

44. The next step is to add beam members along the edges of the slab to represent the upstand. This is done by clicking on “Sub Model Members” in the navigation window which opens the Define Sub Model Members form so that additional members can be created.

45. In the graphics window click on the toolbar button to draw a single member . Then click on the bottom left corner node of the mesh and then again on the bottom right node to draw one member.

46. Repeat this on the top edge of the mesh. These members can then be split into 20 beam element segments by using the Split Beam Element task in the Define Sub Model Members form.

    

47. In the split beam elements form select the 'at nodes along element option', click on the edge beam and then click on the Apply button.

48. Dismiss the information window and repeat for the beam on the top edge of the mesh and then close both forms with ✓ OK.

49. At this stage it is worth saving the slab model as an intermediate data file so that we can come back to this stage if necessary. Close all the open forms in the normal way and save the model as “My EU Example 10_2 Slab.sst”.

    Creating the curved slab

    The next step is to alter the z coordinates of the slab nodes to represent the curved profile. To do this the 2D sub model needs converting to a 3D sub model (losing all details of the mesh).

50. This is done by clicking on the sub model in the navigation window and, by using the right mouse button, choosing the menu option Convert to 3D sub model.

51. Confirm the conversion when asked.

52. Open up the Joint Details form by clicking on this item in the Navigation Pane and ensure the view direction is a plan view.

53. Draw a selection window round the left most transverse row of joints to select them. These joints will be displayed as red.

54. Hold the “Ctrl” key down and draw a selection window round the right most transverse row of joints to add these to the selection set.

55. Click on the Edit... joint task to display a secondary form to allow editing of the coordinates.

56. Choose the Specific value option and enter “-1.000” in the Z field before clicking on the “Apply” button.

57. Without closing the Edit Joint Coordinates data form, select the second column of joints from each end in the same way as before, and change the z coordinate to “-0.810” before clicking the “Apply” button.

58. Repeat this with appropriate Z values (given in the table) for the other columns of joints.

59. Close the Edit Joint Coordinates form and use the graphic toolbar button to set the view as isometric.

60. Close the Joint Details form in the normal way.

Row of joint	Z Coord (m)
1	-1.000
2	-0.810
3	-0.640
4	-0.490
5	-0.360
6	-0.250
7	-0.160
8	-0.090
9	-0.040
10	0.000
11	0.000

Before moving away from the curved slab geometry it is worth checking the local axis directions of the finite elements and beams as the rules for elements not in a global plane are different to those that are.

61. Click on the General button on the right side of the graphics window and tick the Local Axis box. Some of the finite elements may have different direction to the others, depending on the order in which they were generated, and to ensure that any propertied assigned and results output are sensible then it is necessary to make them consistent.

62. In the Structure Definition navigation window, first click on Structure and then use to add an Advanced FE set | Local Axes which will open the Specify FE Local Axes Set form.

63. Type should be set to “by Plane” and Orientate Element w.r.t. set to “Plane XY”.

64. Window round the entire slab in the graphics window to apply this to all the finite elements and then in the Confirm form select “Yes to All” and then close the data form with ✓ OK.

    The deck slab geometry is now complete so a design line, carriageway and span end lines can be added to the structure definition. The local axes display can now be turned off if required.

65. In the navigation window click on Structure and use the toolbar button and select Design Line to open the Define Design line form. The structure will be displayed in an xy view.

66. Click on the middle node at the left hand edge of the structure, then on the middle joint at the right hand edge of the slab to create a design line “DL1”.

67. Click on ✓ OK to close the Define Design Line form.

68. To create the carriageway use the button (when Structure is highlighted) and select Carriageway.

69. In the Define Carriageway form set the design line to “DL1” and change the offsets to +/- 1.9m on either side of the design line for both footway and carriageway.

70. Click on ✓ OK to close the Carriageway form.

71. The two span end lines are added in a similar way and are best created by opening the Span End Lines form, inserting two rows in the table and entering the four coordinates manually (0,0) (0,4) (30,0) (30,4).

72. Click on ✓ OK when the span end lines have been defined.

    

73. Close the data forms in the normal way and save the data file as “My EU Example 10_2 Curved Slab.sst”.

    Assigning the composite beam

74. In the Structure Definition navigation window click on the button and select FE Web from the list. To allow cracked concrete properties to be assumed in the end hogging regions of the slab, the field Proportion from left/right can be entered at “0.06” (i.e. just over one element).

75. Set Name to “North Girder”, change to a plan view and click on the bottom edge of one of the top row elements.

76. Accept the two information messages.

77. Click on the Add Additional FE Web... button (accepting the information message about aspect ratios) and tick the Mirror Design Beam button.

    

78. Set Name: to “South Girder” and click on the top edge of one of the bottom row elements and accept the information message, then close the form.

79. Click ✓ OK on the Define FE Web form and accept the information message about aspect ratios.

80. There should be no changes to be made but, it is worth inspecting the section properties that have been created in the process of assigning FE Web members by using the Structure Properties navigation window.

81. In the Structure Properties navigation window click on the button and select Design Section to open the Structure Properties: Section data form.

82. Select a Section Reference of “Edge Upstand”, the Section Reference Axis Relative to to “Origin” and then window round both the north and south edge of the structure before closing the form with ✓ OK.

83. Use the main menu File | 3D Elements View to view a 3D representation of the structure as it stands.

    It should be noted that the upstand on the south edge of the structure is not situated correctly in a lateral position. To rectify this, a longitudinal beam (string of beam elements) can be created for this edge and then reversed.

84. In the Structure Definition navigation window select Longitudinal Beams to open the Longitudinal Beams form.

85. Window round the south edge beam, to create a longitudinal beam between span end lines, and then in the Beam Tasks click on Reverse Order to change the direction of the local axes of these beams. Now the 3D elements view will show the corrected location of the edge beams.

86. The next step is to modify the virtual members, created when the FE webs were defined, to include the upstand edge beam members. To do this, go to the Calculate | Define Virtual Member menu item.

87. Change to a plan view and make sure the pick mode is set to “Beam Element”.

88. Select “_FE Web A_” and draw a box around the top edge of the slab.

89. Repeat the process for “_FE Web B_”, selecting the bottom edge.

90. Rename “_FE Web A_” and “_FE Web B_” to “North Girder” and “South Girder” respectively, by selecting and overtyping.

91. Then close the Define Virtual Member form with ✓ OK.

    Adding the Pile and Diaphragm Sub Models

    The next step is to define the pile and diaphragm sub models which can be achieved by creating a 2D sub-model in the vertical plane along the east abutment. This can then be copied to the west abutment.

92. In the Structure Definition navigation window toolbar click on the button to select 2D Sub Model and click on the YZ button then click ✓ OK.

93. Click on “Sub Model Members” in the 2D Sub Model: 2D Model A object to open the Define Sub Model Members form.

94. Click on the Single Member draw mode toolbar button () and click on the bottom left hand node on the beam web.

95. Click on the Draw to a specific position or offset toolbar button () then click on the Offset value button.

96. Enter a v offset of “-4m”.

97. Repeat the process to define the other pile.

98. Click on Split Beam Element from the list of Member Tasks then click on the by specified divisions button, set the number of new elements to 8, then click on the “Apply” button.

99. Click on the first pile and click on the “Apply” button again, then close both the forms.

100. Click on 2D Sub Model: 2D Model A in the navigation window then click on the to select “Mesh” from the drop down list.

101. Set the Member type to “Finite Elements”, the Transverse Number to “2” and the Longitudinal Number to “4”.

102. Set Pick to “by point”.

103. On the graphics window put the mouse on the General tab and tick the Show Nodes option. The nodes will show up as blue dots.

104. Set the Snap mode to “Node in Plane” and click on the 4 nodes highlighted in the screenshot below, starting with the bottom left then bottom right, top right and top left. This will create a finite element mesh.

     

105. Change the Name to “Diaphragm” and close the Define Sub-Model Members form with ✓ OK and clicking “Yes” on the confirm form.

106. In the Structure Properties navigation window click on the button and select Design Section to open the _Structure Properties: Section _data form.

107. Select a Section Reference of “H Pile”, and set the Section Reference Axis Relative to: to “Origin”; then window round the whole structure. This will try to apply this section to all beams in the structure, so select “No to All” when asked if beams already assigned should be overwritten. This will ensure that only the pile members will be assigned.

108. Close the form with ✓ OK.

109. Click on the toolbar button again and select Finite Element from the dropdown list.

110. Set Thickness to “500mm” and then select the 8 finite elements in the diaphragm.

111. Change Description to “Diaphragm" and close the forms.

112. In the Structure Definition navigation window use the button to add Supported Nodes.

113. Change the Select field on the graphics toolbar to “All Joints” and click on the two bottom nodes of the piles.

114. Fix the joints in all six directions then click ✓ OK to close the form.

115. The next step is to copy the sub model to the other end of the structure. Right click on 2D Sub Model: 2D Model A and select “Copy” from the popup menu.

116. Click on the Define button and set X to be “30m”, leaving Y and Z at their current values.

117. Click on the “Next” button 3 times on the Define Plane form and then the ✓ OK button.

118. Click on the “Next” button on the Copy Sub Model form to copy the sub model. A summary of the new members, elements, joints and supports created is then displayed.

119. Click on ✓ OK to close the Copy Sub Model form.

120. Click on the Show advanced model view icon () to view the elements of the structure in a 3D representation. Clicking on the Object Browser tab below the Navigation Pane and selecting an element in the graphics window displays detailed information about that element in the space that is normally occupied by the Navigation Pane. Note that unless the Filter is set to “Select all” then not all of the members will be rendered in the 3D representation.

121. Save the file as “My EU Example 10_2 Full Structure.sst”.

     Adding Dead and Superimposed Dead Load

     The next step is to define the dead and superimposed dead loads.

122. In the Structure Loads navigation window click on the toolbar button and select Beam Member Load | Beam Element Load from the drop down list.

123. Click on the () toolbar button then click on “De-select all”. Set Select By to “Structure Property” and add “Steel Flanges”, “H Piles” and “Steel Web” to the Selected Groups list.

124. Click on the “Save” button and save the member selection as “Steel only” before closing the Member Selection Filter form.

125. Change Direction to “Global Z” in the first row of the table, Load Value to “Volume”, Load W1 to “-77” and the Name to “Steel Dead Loads (Beam)”.

126. Draw a box around the entire structure before closing the Define Beam Loading form.

127. Click on the toolbar button and select “Finite Element Load | External Load”.

128. Change the Load Type to “Force/volume”, Direction to “Global Z”, Load to “-77” and Name to “Steel Dead Loads (FE)”.

129. Draw a box around the entire structure and then close the Define Finite Element Loading form.

130. Click on the toolbar button and add another Beam Member Load | Beam Element Load.

131. Click on the () toolbar button and de-select all.

132. Set Select By to “Structure Property” and add “Edge Upstand”, “Cracked Slab”, “Slab” and “Diaphragm” to the Selected Groups.

133. Click on the “Save” button, and save the selection as “Concrete Only” before closing the Member Selection Filter form.

134. Change Direction to “Global Z”, Load Value to “Volume”, Load W1 to “-25” and the Name to “Concrete Dead Loads (Beam)”.

135. Draw a box around the structure to select all the concrete beams before closing the Define Beam Loading form.

136. Click on the toolbar button and select “Finite Element Load | External Load”.

137. Change the Load Type to “Force/volume”, Direction to “Global Z”, Load to “-25” and Name to “Concrete Dead Loads (FE)”.

138. Draw a box around the entire structure and then close the Define Finite Element Loading form.

139. The next step is to define the dead load compilations. In the Structure Compilations navigation window, click on the button and choose “Dead Loads at Stage 1”.

140. Set the Limit State field to “ULS STR/GEO” and then click on the Find and Add to Table button to populate the table. The gamma factors for the Steel dead loads will need changing to “1.2”.

141. Set the name to “DL ULS” and close the form.

142. This process needs to be repeated for SLS. Click on the button and choose “Dead Loads at Stage 1”.

143. Change Limit State to “SLS Characteristic” then click on the Find and Add to Table button.

144. Set the name to “DL SLS” and then close the form.

145. The next step is to define the superimposed dead loads. In the Structure Loads navigation window toolbar click on "+" and select “Bridge Deck Patch Load”.

146. Change Define Loading by to “coordinate” and Load per unit area to “2kN.m²”.

147. Change Snap mode in the graphics window to “Intersection” and click on the four corners of the deck to define the patch (the original point needs selecting again at the end).

148. Change Name to “Surfacing” and then close the form.

149. In the Structure Compilations navigation window click on the toolbar button and select “Superimposed Dead Loads”.

150. Set the Limit State field to “ULS STR/GEO” and then click on the “+” button to add a new line.

151. Click in the Load Name drop down list and select “L5: Surfacing”..

152. Set the name to “SDL ULS” and close the form.

153. Right-click on “C3: SDL ULS STR/GEO” on the Navigation Pane and select “Copy”.

154. Change Limit State to “SLS Characteristic” and answer “Yes” when prompted to change the factors.

155. Change the name to “SDL SLS” and close the form.

156. Use the Member selection filter function to select all members.

157. Save the file as “My EU Example 10_2 Dead and SDL.sst”.

     Automated Loading Using Influence Surfaces

     The next step is to create a bending moment influence surface for a particular point on the south girder and generate a live load pattern that will produce the worst effect.

158. To do this, select the Data | Influence Surface menu item.

159. Set the Pick Mode to “Virtual Member Element”.

160. Change the graphics view to plan and click on the location indicated by the arrow below:

     

     This will add virtual member element 2-11 to the list of influence surfaces to be generated.

161. Set the Method field to “(1) Smoothed”.

     

162. Click on the Analyse button to create the influence surface. When the analysis is completed the influence surface will be displayed on the graphics.

     

163. Click on the “Done” button.

164. Set Type to “Road Traffic” and then click on the Run Optimisation... button to open the Road Traffic Load Optimisation to BS EN 1991-2-2003 (UK Annex) form.

165. In the Groups and Limit States list ensure that only “gr5” in both the ULS STR/GEO (B) and SLS Characteristic sections are ticked.

166. In the Load Model 3 Special Vehicles field tick “SV80”.

167. Click on the Compile Loading Patterns button to run the load optimisation.

     

     Details of the load optimisation run will be shown together with the loads created both on the form and in the graphics window.

     

     Click on ✓ OK on the load optimisation and influence surface generation forms to save the loads that have been created.

168. It is now necessary to analyse the load cases that have been created. In the main menu select Calculate | Analyse Structure, which will open the Activate Loading Sets form. Each run of the load optimisation will create its own loading set, so this form can be used to select which load optimisation runs we want to produce results for.

169. In this case there is only one run so leave the form as it is and click ✓ OK which will start the analysis and progress will be displayed in a status box.

170. When the analysis is complete click on the ✓ Done button.

     

171. Save the file as “My EU Example 10_2 Dead SDL Influence.sst”.

     Transfer analysis results to the beam design module

172. The next step is to transfer the results of the analysis to the appropriate design beam which can be done by selecting the Calculate | Transfer Results menu item. This will open the Transfer Results form.

173. Click on the graphics window anywhere along the reference axis of the south girder to highlight the virtual member that will be used to determine what results will be transferred to the design beam tables.

     

     The selected beam will be highlighted and its details shown in the Transfer Results form.

174. Click on the “+” button at the bottom of the table to create six blank rows of data. The Method field should be set to “(1) Smoothed” for this example.

175. Click in the first row of the Design | Load Case column and select “Construction stage 1”.

176. Click in the Type column and select “Compilation”.

177. Click in the Structural Analysis | Load Case column and select “C1: DL ULS”.

178. Repeat the process in the second row, this time setting Structural Analysis | Load Case to “C2: DL SLS”.

179. In the third row set Design | Load Case “Surfacing 1”, Type to “Compilation” and Structural Analysis | Load Case to “C3: SDL ULS”.

180. Repeat the process in the fourth row, this time setting Structural Analysis | Load Case to “C4: SDL SLS”.

181. In the fifth row, set Design | Load Case to “Traffic gr1b-gr5 +ve Moment 1”, Type to “Compilation” and Structural Analysis | Load Case to “C5: VM2-11; My Sagging; GR5 ULS STR/GEO”.

182. Repeat the process in the sixth row, this time setting Structural Analysis | Load Case to “C6: VM2-11; My Sagging; GR5 SLS Characteristic”.

     The table in the Transfer Results form will now look like this:

     

183. The Current Set can now be transferred to the EU steel composite design beam by using the Transfer Results button.

184. The composite Design Beam can then be checked that the beam has sufficient resistance under all loads in a similar way to the procedures defined in example 5.1.

185. When all design checks have been completed the project file can be saved to a file named “My EU Example 10_2 Complete.sst” before closing the software.