SolidWorks 2011 Parts Bible - Matt Lombard [54]
• Automatic Solve is turned on by default. As you make changes to a sketch by adding relations or changing dimensions, SolidWorks automatically and immediately updates the sketch to reflect the changes. When the Automatic Solve setting is turned off, these changes are deferred until you exit the sketch or turn the Automatic Solve setting back on. The setting can be useful to prevent intermediate solutions (for example, when half of the changes are made) that may cause problems with the sketch, and when you are confident that the outcome will be correct. It is a rarely used option, and you could probably exist just fine without even knowing this option was there at all.
If you import a large drawing from the DXF or DWG format, these drawings import as sketch entities into either a SolidWorks sketch or a drawing. SolidWorks may automatically turn off the Automatic Solve setting for performance (speed) reasons on files of this type.
• Enable Snapping is turned on by default. It enables the cursor to snap to the endpoints of existing sketch entities to help you make cleaner sketches. When you turn this setting off, Automatic Relations is also disabled (although the icon for the setting remains depressed, Automatic Relations are not created). Holding down the Ctrl key while sketching disables snapping. Holding down the Ctrl key while dragging sketch entities functions like copying sketch geometry. The No Solve Move is discussed in the Sketch toolbar section.
• Detach Segment on Drag is turned off by default. When you turn this setting on, the Detach Segment on Drag feature enables you to pull a single sketch element away from a chain of elements. For example, if you had a rectangle and you wanted to detach one of the lines from the rest of the rectangle without using this setting, you would have to draw extra geometry and then trim and delete lines in order to release the endpoints.
Best Practice
It is recommended that you leave Detach Segment on Drag off. Turn it on only when you need it, and then immediately turn it off again. This setting can be hazardous for everyday use, because it enables you to simply drag sketch elements that may be otherwise fully defined.
• Override Dims on Drag is off by default. When you turn this setting on, it enables you to drag fully defined sketch geometry, and the dimensions will update to match the dragged size. This is another setting that you should use sparingly. It can be useful for doing concept work, but you should leave it off when working with production data for obvious reasons.
Note
Combining Override Dims on Drag with Instant3D can be very handy for concept work, enabling you to drag sketches, model faces, and edges easily.
Using Sketch Blocks
Sketch blocks are collections of sketch entities that can be treated as a single entity and can be reused within a single document or shared between documents. You can use sketch blocks in parts, assemblies, and drawings. To create a sketch block, select a group of sketch entities and click the Make Block button on the Blocks toolbar, or select Tools⇒Blocks⇒Make. Pre-selection is not necessary; you can also select the entities after you invoke the command.
Blocks may be internal to a particular document, or they may be saved as an external file. The externally saved block may be linked to each document where it is used, so that if the block is changed, it updates in the documents where it is used.
You can use blocks in conjunction with the Make Path function mentioned earlier in this chapter to create functional layouts for mechanisms. You can also use blocks in an assembly to build parts in-context. Refer to the SolidWork 2011 Assemblies Bible (Wiley, 2011) for a more in-depth examination of the assemblies aspects of blocks in SolidWorks.
The following is a description of the various