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Make sure the holes are Counterbored, ANSI Metric, Socket Head Cap Screw, M10, with a head clearance of 0.10 inch. All other conditions should follow Figure 6.9.

10. Place two more new holes on the other side. Make the parts transparent to see how the holes have been placed.

FIGURE 6.10

Placing screw holes through multiple parts in the die

11. Initiate the Plane feature. Create a plane perpendicular to the Right plane and coincident to the line from the Plate Depth Layout shown in the Right view in Figure 6.11. Rename the new plane Sprue Bushing Seat. (The new plane should show up right underneath the initial three layout sketches.)

12. Create a new part on the Sprue Bushing Seat plane.

FIGURE 6.11

Creating a plane in the assembly driven by the layout sketch

13. Activate the Convert Entities sketch tool, select the large (approximately 4-inch diameter) circle from the Pin Layout sketch, and convert it into the sketch plane of the new part.

14. Draw a 1/2 inch circle in the center (at the origin). Extrude the sketch 0.875 inch so that it protrudes from Plate 2.

15. Exit the Edit Part mode (using the Confirmation Corner). Rename the new part Sprue Bushing.

16. Left-click on Plate2 and select Edit Part from the shortcut toolbar.

17. Open a new sketch on the Sprue Bushing Seat plane (which is part of the assembly, not part of the part).

18. Select the large circle used in Step 13, and use the Offset sketch tool to offset the circle 0.005 inch to the outside. Create a Through All cut that comes out the exposed side of Plate2, clearing an area for the Sprue Bushing. You may need to switch to Wireframe display to accomplish this.

19. Apply a chamfer to the outer edge of the new cut, 0.010 inch.

20. Exit Edit Part mode, and save the assembly to a new location by choosing File ⇒ Save As. Click the Save All button, and then select the Save Externally option, as shown in Figure 6.12.

FIGURE 6.12

Saving the internal virtual components to external parts

21. Exit Edit Part mode using the icon in the Confirmation Corner.

22. Double-click the Plate Layout sketch, and change the 5.836 inch dimension to 6 inches. Change the 7.244 inch dimension to 7 inches. Make sure the model rebuilds, and watch the individual parts update. Figure 6.13 shows these dimensions for reference.

FIGURE 6.13

Editing layout sketch dimensions to drive the size of the individual parts

You will need to do more to finish this tooling die than is covered in this tutorial. The point is to give you some experience using the in-context features that are used with a layout sketch technique.

Summary

Laying out an assembly with reference sketches is a more disciplined way of working that can help you avoid some of the complications of external references and in-context design work. It is up to you to decide whether the informal 2D layout sketches are preferable to the formal 3D sketch-based Layout feature. Both offer tools to control positions of parts and even features of parts within an assembly.

Traditional assembly modeling methods where each part is located by mates from another part do not stand up well against changes in the parts themselves. The main goals of the layout methods are centralization of control and stability of changes. I invite you to explore some of these methods using tools you have learned in this chapter.

Chapter 7: Using Assembly Tools

In This Chapter

Assembling without mates

Interfering options

Using AssemblyXpert

Defeaturing in assemblies

Using sensors

Aligning holes

Working with large assemblies

SolidWorks assemblies enable you to take advantage of several tools in addition to the standard and best-known functionality. The tools covered in this chapter didn't fit into other chapter headings easily, but deserved significant coverage.

Placing Parts without Mates

Assembly mates are great tools, but they aren't the only tools for placing parts in an assembly. Sometimes