DRAFT OF DEMO FOR The following set of instructions are an optional replacement for the Section Views in SolidWorks. This demo should help prepare the students for the Out of Class HW Student + Instructor: 1. Click on the files on the EEIC website containing the Sections.SLDPRT and the Sections.SLDDRW and place both on the Z drive. Open SolidWorks and using File / Open, bring both the part and the drawing into SolidWorks. Select the drawing for display, maximize the window and then use Zoom to Fit maximize the image. 2. The drawing is organized to be discussed from top to bottom and right to left for the Full and Half sections: Discuss the "Use Section Views" text and then the "Section Views Components" Discuss the "Full Section" noting the 3 labeled components( red/orange/blue) Discuss the "Full Section" crosshatching and the section label, noting that if SCALE information appears, it should be removed (in title block). The section line is drawn within the Section View function as will be demonstrated later. Discuss the "Half Section" noting that you need to activate the "Sketch" to draw the desired section lines. Before selecting "Section View" in "View Layout", with the Ctrl key depressed, the student needs to select first the vertical line and then the horizontal line to force the section view to be generated in the downward direction. Reversing the order will produce a side section view. 2 1 Left click on the screen in the area of the "OFFSET" section view new the bottom of the drawing and zoom in using the mouse wheel. Discuss the application of the offset section view when the desired features cannot be sectioned using a straight section lines. Note that where the offset section line creates a cut through solid material (see the vertical section lines),
that cut does not produce a solid vertical line in the drawing since such a line would be confusing to the viewer. Use Zoom to Fit to restore the full drawing view. Repeat the previous step for Broken, Revolved and Removed sections. Note that in the Revolved and Removed sections, the cutting plane is perpendicular to the element being section, but the produced section view is rotated 90 degrees prior to placement in the drawing. 3. This concludes the discussion of the drawing which should now be deleted from SolidWorks. 4. With the part file still resident, click on File / New / OSU Title Block to bring in a blank drawing page. 5. Under View Layout, select Model View and browse for the part file. When located, double left click on the file and in the dropdown window select Top View, move the mouse to the right and place the outline of the part in the upper right portion of the screen, left click to place and hit Esc key. 6. Select Section View / Section View and move the pencil icon to the RIGHT of the part image and hover / hunt for the extension of the horizontal center line as shown. WARNING: If drawn from the left and pulled down, the section view will be upside down and the arrows will point downward If 7. Once located, left click to start the section line and then move the mouse left across the object to just beyond the left side and left click again keeping the section line horizontal and intersecting the center point of all the holes. Move the mouse downward to position the section view below the top view and left click to fix it s location.
8. Select Annotation / Centerline and sequentially left click on the left and right sides of all the holes and finally accept the Centerlines by clicking on the green arrow or by hitting the Esc key. The Full section is now complete. 9. Select Layout / Model View and open another copy of the part by double clicking on the file followed by clicking on the top view in the drop down dialog box and moving the mouse to position the image adjacent to the Full section. Left click and hit the Esc key to fix the top view. 10. Select Sketch Line / Line and carefully draw a horizontal line From just to the right of the part in line with the center point of the small hole to the center point of the large hole. Hit the Esc key to accept. Repeat the above sequence and draw a Vertical line from the center point of the large hole to just Below the part and hit the Esc key to accept. 11. First select the vertical line. Holding the Ctrl key down, select the horizontal line. Both lines should turn blue. Select View Layout Section View / Section View and with the mouse pull the section view down below the top view and left click to position and hit the Esc key or the green arrow to accept. Note that the hidden lines are still visible in the left side of the section. Select Annotation / Centerline and left click on the left and right side of the small hole to create the center line. Repeat for the large hole. Note short centerline.
12. To make the center lines of equal length, click on the Screen near the center line of the large hole and zoom in using the Mouse wheel. Click on the center line to show the small blue Squares designating the extremes of the center line sequentially Pull each box away from the object and then reposition so that the lengths are the same. Reposition drawing using "Zoom to Fit". 13. To remove the hidden lines on the section view left click on Section B-B and then select Display Styles / Hidden Lines Removed and hit the Esc key or select the green arrow to accept. Even though we placed two placed two different sections on the same drawing for this demo, one would not do this for a standard section view drawing. Note that the convention followed by SolidWorks is slightly different due to the extra arrowhead and the line direction on the Half section. The standard used by our text would have the vertical line straight down without an arrowhead (shown in blue) to clearly show the view direction. We will not fill out the required title block in this demo. Since this object is symmetrical, a third view (right side) would not provide any new information and is not necessary. Remind the students that there is a Sections Demo Results drawing file ( identical to the above figure ) on the EEIC website which can be referenced by the students if they do not complete the in-class demo.
14. (Use steps 14 & 15 or discuss the in class assignment on the EEIC website)edit the title block and complete as shown with the students adding their personal information. The title block is accessed by right clicking anywhere in the drawing area and selecting "Edit Sheet Format". Return to the drawing is accomplished either by right clicking anywhere in the drawing area and selecting "Edit Sheet" or by left clicking on the icon in the upper right corner. 15. Select Zoom to Fit, print and submit object as optional in class assignment.