SolidWorks 2011 Assemblies Bible - Matt Lombard [58]
In practice, this feature needs some enhancements before it is ready for use on real assemblies. Using 2D sketches as assembly layout sketches may still be a better idea than trying to avoid the following limitations of the formal Layout feature:
• The 3D sketch used for Layout has all the limitations that come with 3D sketches.
• Sketch relations are listed in the Mates folder.
• Gaining access to edit the Layout once it has been closed requires a method you don't expect from a sketch: you click the Layout button on the toolbar rather than right-click and edit an icon in the FeatureManager.
• It requires that you use blocks to access all of the functionality.
• A fully defined 3D sketch with blocks is very unstable.
• Part creation from blocks does not save time.
• You cannot paste copied sketch entities from a 2D sketch into the Layout.
• You cannot use sketch pictures in the Layout.
• You cannot use auto-dimension (or polygons or ellipses) in the Layout.
Although the formal Layout feature has serious advantages over regular layout sketches, at this time the limitations outweigh them. The rest of the discussion on layouts addresses the generic layout technique rather than the formal feature.
Tutorial: Working with a Layout
In this tutorial, you will use regular assembly sketches to lay out and build a tooling die.
1. Open the assembly from the DVD named Chapter 6 tutorial layout start.sldasm. Notice that three layout sketches and some of the parts have been added already. The existing parts are virtual components, saved inside the assembly.
2. Click Add New Part on the Assembly tab of the CommandManager. The cursor appears with a green check mark, and in the lower-left corner, the taskbar prompts you to select a plane on which to place the Front plane of the part. A sketch will automatically be opened on that plane. Click the Front plane of the assembly.
3. Click the Corner Rectangle sketch tool from the Sketch toolbar. Create a rectangle from the two corners indicated in Figure 6.8. It may be helpful to bring the model into a Front view before drawing these rectangles.
4. Extrude the rectangle using the Up To Vertex end condition for both Direction 1 and Direction 2. Select sketch endpoints in the Plane Depth Layout sketch for both directions so that the new plate matches the other existing plates.
Be careful not to click model faces, edges, or vertices when creating these depth references. Make sure that all your references stay in the sketch.
FIGURE 6.8
Creating a new plate in the context of an assembly with layout sketches.
5. Click the Exit Edit Part icon in the Confirmation Corner (the upper-right corner of the SolidWorks graphics window). Right-click the new part in the FeatureManager and select Rename Part. Rename it Plate4. You can also use the Windows standard method of slowly double-clicking rename parts. The Chapter 16 tutorial layout start part of the name is automatically added. Assign a material from the Appearances tab for the new plate.
6. Follow this procedure for the four remaining plates, as shown in Figure 6.9. To summarize the steps again, you add the new part, create a sketch, and extrude the block.
Note
Be careful with the plates labeled 5, 6, 7, and 8. There is a clearance gap between the sides of the 7 and 8 plates and the vertical plates 5 and 6.
FIGURE 6.9
All of the plates controlled by the layout sketches
7. Reorient the view to the Top view. Make sure you can see the Pin Layout sketch.
8. Select the top face of Plate 1, and click on the Hole Series toolbar. The Hole Series may be hidden under the Assembly Features flyout on the Assembly tab of the CommandManager. The Hole Wizard no longer requires pre-selection to avoid 3D placement sketches, but the Hole Series as of 2010 has not been updated to follow the same rules as the Hole Wizard.
9. Place two sketch points at the centers of the circles, as shown in Figure 6.10. Make sure that the two points are both over the same plate 5 or 6. You cannot cut both plate 5 and