SolidWorks 2011 Parts Bible - Matt Lombard [237]
SolidWorks has a toolbar just for the alignment of dimensions and annotations. The toolbar is shown with labels for individual icons in Figure 17.18. To add the Align toolbar to the CommandManager, right-click one of the CommandManager tabs, and select Customize CommandManager. Then click the new tab that appears and select the Align toolbar from the list.
FIGURE 17.18
Using the tools from the Align toolbar
Using the alignment tools
The alignment tools are all pre-select tools, and so it is best to box-select (or Ctrl+select) the dimensions and annotations you want to align first, and then click the toolbar icon. For example, to align a set of balloons to the right, you would drag a box around the balloons, Ctrl+select any balloons you could not select with the box, and then click the Align Right button. These tools work best with larger selections of dimensions or annotations. For aligning individual dimensions or pairs of dimensions, it might be better to use the drag methods discussed in the section “Inferencing alignment and grid snapping.”
Using the alignment tools Align Collinear/Radial and Align Parallel/Concentric creates persistent relationships, so those dimensions aligned with the tools will maintain that alignment. The other tools on the Align toolbar do not work this way. To break an alignment created by these tools, select Break Alignment from the RMB menu.
Using the Group tool allows a set of dimensions and annotations within a single view to maintain the spatial relationships for dimensions that were not aligned with the alignment tools, until they are ungrouped.
Inferencing alignment and grid snapping
When you drag individual dimensions on a drawing, they are snapping to a grid. (Annotations do not snap to the grid.) This is one way that SolidWorks helps you to align them. If you drag one dimension level with another, either horizontally or vertically, a line appears and the dimension inferences the position of the other dimension, just like lines snapping in model sketches.
Annotations will inference other annotations, but they won't inference dimensions, and they won't snap to the grid.
If you want to disable both kinds of snap (grid and inference) on the fly, just hold down the Alt key while dragging, and the dimension or annotation will slide freely. To permanently disable the snapping, go to Tools⇒Options⇒Drawings⇒Disable Note/Dimension Inference. To disable the snap, make sure this option is selected. You should be aware that this option controls both the snap to the grid and the inferencing of one dimension or annotation to another. You cannot separate the grid from the inferencing.
If you like the snaps and want to change the spacing, you can do that by selecting Tools⇒Options⇒Document Properties⇒Dimensions⇒Offset Distances and changing the appropriate numbers for the distance of the dimension from the edge of the part and the distance between dimensions.
If you are used to older versions of SolidWorks, you will remember that the snapping used to depend on where you selected the dimension — from the top, middle, or bottom — and it would line up with other dimensions using the same references. Newer versions of SolidWorks are more simplified, and I think they work better.
If you want a group of dimensions or annotations that you have aligned to maintain their current alignment, box-select them and use the Group function from the Align toolbar. All of the selected dimensions and annotations must belong to the same view.
Using Dimension Palette alignment options
The Dimension Palette, mentioned earlier in this chapter, enables you to surround a dimension with all of the necessary information, such as additional text, tolerances, symbols, justification, leader control, dual dimension display,