Creating Hourglass Spring with Solid Edge ST

In this tutorial you learn: • How to model an hourglass shaped spring in Solid Edge synchronous design mode. • How to use the Bluesurf command. • The use of swept surface. • How to intersect surfaces to make 3D curves. • How to use the steering wheel in the synchronous mode in Solid Edge.

A full index of Solid Edge surfacing tutorials on this blog is here.

Disclaimer:
• This tutorial and the steps illustrated herein are by no means claimed to be the best or the only way to create the given design.
• This tutorial is an attempt to introduce and demonstrate the awesome set of tools that Solid Edge has for curve creation and surface manipulation.

Start with a new ISO part by clicking on the Solid Edge Application Button > New > ISO Part. On the Ribbon bar, take the Tools tab and from the Model group, select Synchronous. The feature PathFinder updates to reflect this. Start Line and hover the mouse over one of the vertical planes - Right (yz) or Front (xz)
When the plane highlights, click over the small lock icon as shown in image to lock the plane for sketching. Draw a vertical line 100 mm beginning from the Origin. Key-in 100 in the Length box on the Command bar and move the cursor.
A pink line starts appearing as you move the cursor. Move the cursor till you see the vertical alignment/relation symbol as shown circled in image besides. Together, these ensure you have drawn a 100 mm vertical line in the xz Base Reference Plane. Click to place the line, then click the Unlock icon to unlock the sketching plane.
Similarly, draw a Rectangle by two Points in the Top (xy) plane. Key-in the Width as 50, height as 2 and Angle 180 Apply a Smart Dimension if required. Your sketch should now look as shown.
From the Surfacing tab, Surfaces group, select Swept   For the Path step, select the vertical line. Click Accept on the Command bar. For the Cross Section step, select the rectangle.
Don't Finish the Swept command yet. Click Sweep Options on the Command Bar and in the Twist area, specify Number of turns as 12. Click OK in the options dialog and Finish the Sweep command. The surface should form as shown.
From the feature PathFinder, check OFF the Sweep1 surface to hide it. From the Sketching tab, Planes group, select Coincident Plane and select the Top (xy) Base Reference Plane from the PathFinder. A new plane appears with the Steering Wheel active.
Drag the vertical primary axis of the steering wheel 50 mm up. Similarly, create another plane parallel to the last created plane at distance of 50 mm above. Start Circle and lock the Top (xy) Base Reference Plane for sketching. Set the circle diameter to 100 and centered about the Base.
On the middle plane, draw a concentric circle of diameter 50 mm. On the top-most plane draw another concentric circle of diameter 100. Use Ctrl+T or Ctrl+H to switch to the Sketch View.
Start BlueSurf and select the three circles in proper order to create the BlueSurf as shown. Next Check ON the Swept surface from the PathFinder and start Intersect from the Modify Surfaces group of the Surfacing tab. Select the Swept surface and the BlueSurf one after another and click Accept
In the Trim and Extend Step, select the two surfaces of the swept surface formed by the far and near sides of the rectangle's shorter side.   You can use the QuickPick to choose the surfaces needed. Click Accept and the resultant trimmed surface should look like as shown in image.
Hide the Swept surface again and you should see whatever is left of the the BlueSurf - a thin sliver as seen in image besides. Start Derived Curve from the Curves group of the Surfacing tab. Pick an edge of the BlueSurf to create the curve.
Hide the BlueSurf too and all that is seen is the derived curve - a path for creating a Swept protrusion. Create a a Plane Normal to Curve by picking the derived curve first and then one of its endpoints.
Create a Circle in the new plane with its center at the pierce point of the curve with the plane. From the Home tab, Solids drop button, start Swept Protrusion and use the derived curve as path and the circle as cross section to create the spring in the shape of an hourglass.
Using similar technique, various springs like square spring, square tapered spring and star spring can be created. To create square tapered spring create a BlueSurf between two rounded squares or rectangles as shown besides and intersect it with the helical or twisted surface. The other steps remain identical.
To create a star shaped spring, create a BlueSurf using star sketches. The Polygon command can prove to be very useful in drawing star shapes, in that, draw two concentric hexagons of different sizes and draw a curve connecting alternate midpoints and corners of the hexagons as illustrated below.

An ordered version of this tutorial is in order with no pun intended, so bookmark this page and visit next week again.

Equally simple and interesting is creating your own, brand new, fully functional CAD system with 3D sketching and surfacing capabilities using a geometric modeling kernel. cMayoCAD from CADVertex is one such program. Download detailed course contents for cMayoCAD here.

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