Creating Point-to-Point Shapes

This task shows you how to create more shapes to complete the structural frame of your foundation. This second series of shapes will all be created using the point to point method. To help define points, you will use the Point Definition command.
1.	Double-click the Shape icon. The Shape dialog box appears. If needed, click the right-hand icon in the status bar to show the Point Definition dialog box.
2.	Set the Type to Point to point in the Shape dialog box.
3.	Click Point on member in the Point Definition dialog box, then select the appropriate shape, at the end nearest to which you want to create the current shape. The Start and End points of the section are identified in the geometry area; an offset of zero with respect to the selected end is displayed. An offset field also appears in the Point Definition dialog box.
4.	Enter an offset of -200mm in the Point Definition dialog box, then click `OK`.

You can offset from the end of a shape in two directions by entering a negative or positive value. If you enter a negative value, the offset will be applied toward the center of the shape. In the image above, the offset point displays closer to the center. If you enter a positive value, the offset will be in the other direction - away from the center.
5.	Define the other end of the shape by entering X,Y,Z coordinates (0, 1300, 0) in the Point Definition dialog box. The shape is positioned but not yet correctly oriented.
6.	In the Shape dialog box, set the Anchor point to Top right and enter an orientation of 270 degrees, then click `OK`.

	You will now create an assembly made of three shapes.
7.	Set the Anchor point to Bottom left and Orientation to 270 degrees.
8.	Select a grid point as starting point, then define the second point 200 mm from this point using the Point Definition dialog box. Note: The coordinates of the selected point are shown in the Point Definition dialog box.
	This is shape 1.
9.	Create the bottom shape using the point-to-point method, with the following criteria: Start coordinate 900, 1500, 300 End coordinate 900, 1500, 0 mm Anchor point: Bottom left Orientation: 180 degrees
10.	Click the Shape icon. The shape (shape 3) you will now create will be defined with respect to points on existing shapes (shapes 1 and 2).
11.	Click the Point on member option in the Point Definition dialog box, then select a first shape at one end of the shape.
12.	Keep the default offset and click `OK` in the Point Definition dialog box.
13.	Click Point on member to define the second point and select the end of the second shape, then click `OK`.
14.	Check the anchor point and orientation and, if necessary, adjust, then click `OK` in the Shape dialog box. Anchor point: Bottom left Orientation: 0 degrees
	You will now trim shapes created to make smooth transitions. To do so, you will need construction geometry to assist you. Construction geometry will be created in a dedicated part. This geometry however must be created without any links to existing shapes since it will also be used to trim these very same shapes.
15.	Uncheck the Keep link with selected object option in the General tab page of the Options dialog box (`Tools -> Options -> Infrastructure -> Part Infrastructure`).
16.	Switch to the Wireframe and Surface Design workbench. A new part is added to the specification tree.
17.	Create two planes offset by 0mm from shape section surfaces of shapes 2 and 3.
18.	Intersect the two planes. The intersect will be used as rotation axis in the next step.
19.	Create a plane at half the angle between the above two planes. This is the plane to which we will trim shapes 2 and 3.
	Use the Measure Between command to measure the angle.

20.	In a new geometrical set (`Insert -> Geometrical set`), create another trim plane as above to trim shape 1 and the other end of shape 3.
21.	Recheck the Keep link with selected object option. You can now trim shapes.
22.	Double-click the root product to return to the Structure Design workbench.
23.	Double-click the Cutback icon. The Cutback dialog box appears.
24.	Select Trim to plane in the Type list.
25.	Select one of the shapes (shape 3) to trim, then the trim plane and click `OK` in the Cutback dialog box.

26.	Repeat for shape 2.
27.	Trim shape 1 and the other end of shape 3 to the other trim plane.

28.	Repeat to create an identical assembly comprising three shapes, starting 200 mm in the Y direction along the corresponding horizontal shape.
		Shape 4: Anchor point: Bottom left Orientation: 270 degrees Shape 5: Anchor point: Bottom left Orientation: 180 degrees Start coordinates: 900, 200, 0 End coordinates: 900, 200, 300 Shape 6: Anchor point: Bottom left Orientation: 0 degrees Note: You can use the same trim planes to trim the shapes of this assembly.