Balloon annotations have been improved in SolidWorks 2014, with several formatting and behavioral enhancements.
Moving the arrow instead of the drawing view
Selection of the geometry within a drawing view tells SolidWorks you want to move the entire drawing view. Normally, this is a great feature. However, there is one case that wasn’t supported as a result. It was not easy to select an arrow which was attached to a vertex of model geometry (because the vertex itself would be selected). In SolidWorks 2014, when moving the arrow of a balloon to attach it to a different location, select the balloon first, then select the grip at the arrow’s tip. This will allow you to move the arrow without moving the entire drawing view.
Leader attachment with quantites added
When a quantity is added to a balloon, the leader is no longer forced to break around the quantity. You now have an option under More Properties button in the PropertyManager of the balloon.
Spacing between quantity and its balloon
You now have control of the distance between the quantity and the balloon with the new Distance field in the Quantity group box of the balloon’s PropertyManager.
You can now reattach any balloon, including dangling balloons within a stack, to associate them with any component from the same drawing view.
Enhancements to Balloons in SolidWorks 2014, together with the enhancements to ballooning in SolidWorks 2013, have improved and simplified many workflows to allow you to produce quality drawings faster and with less effort.
There are many new symbols that have been introduced in SolidWorks since 2012.
New category of Inspection Symbols:
- Inspection Box (empty)
- Inspection Box (with text)
- Eye [for those inspection points that are visual and aren’t/can’t be measured with an instrument]
In addition to new JIS Weld Symbols, these new symbols where added to Modifying Symbols:
- Rho [used with conics]
- Center of Mass
In addition to 5 new JIS weld Symbols, there are several new symbols included in other areas.
- Diamond [alternative for identification of inspection points]
New category View Symbols:
- View Rotation Clockwise (CW)
- View Rotation Counterclockwise (CCW)
- GOST Rotated View
- GOST Unfold
- Translation [including additions to the GD&T interface for compliance with ASME Y14.5-2009]
SolidWorks 2014 introduces the ability to find and use virtual sharps on the on-the-fly while creating dimensions.
- Start any dimension tool.
- Right-click on model or sketch geometry
- Choose “Find Intersection”.
- Left-click on any model or sketch geometry that intersect the first selection.
- The Virtual Sharp element is automatically added, the point is automatically applied as a selection for the dimension tool.
See the attached video below (AVI will open, not an embedded video).
On-the-fly Virtual Sharps (AVI video)
Rob Jost, of SolidWorks Product Definition team, goes into deep detail about the new Style Spline sketch tool now available in SolidWorks 2014, in a recent article posted on the SolidWorks website.
The new Style Spline actually isn’t something new in the world of CAD. It’s an entity that’s been around for a long time, but is sometimes overlooked. It’s called a Bézier curve.
His very detailed article with a tutorial is found here: Style Spline: What is it and why is it useful?
A new type of dimension is now available in SolidWorks called Angular Running which allows you create a set of angle dimensions that originate from a common origin in a style similar to Oridinate Dimensions. Options are available to meet ISO standards, such as adding a chain (dimension lines with direction arrow), and aligned text. Options are also available to apply ASME style rules as well, such as horizontal text. Angular Running Dimensions are added and modified similar to Ordinate and Baseline Dimensions, including the ability to add dimensions to an existing set of Angular Running Dimensions.
Aligned text w/ chain
Inline text w/ chain
Horizontal text w/ chain and bidirectionality
Tables have seen several improvements in SolidWorks 2014. One specifically for BOMs is the ability to save sorts. In previous versions of SolidWorks, sorting BOMs was a one time action. Each time you wanted to sort a BOM, you re-entered your criteria. Not any more. BOMs now have an option that allows you to save your sort by checking the setting called “Save current sort settings” from the Sort dialog. Sort dialog is now available when you right-click on the BOM and select Sort>Custom Sort….
Once OK is selected in the dialog, your settings will be stored with the BOM table. If you make changes to your assembly or the BOM that adds, removes or changes your components, you can reapply your sort at any time by right-clicking on the BOM and selecting Sort>Apply Saved Sort Scheme.
Additionally, when Save current sort settings is employed on a BOM, the settings are remembered when that BOM is saved as a BOM template. This means, on any new drawings, the sort is automatically applied when the BOM template is used to create new BOM!