For drafters that need more control over how dimensions are displayed on their drawings, SolidWorks 2014 has introduced a couple of new controls. First, styles for extension lines and dimension lines can now be assigned independently from each other on dimensions. The default line styles can be set in Document Properties for each dimension type, and within the Dimension PropertyManager.
In the PropertyManager, a new group box has been added, called “Extension Line Style”. Within this group box, there is an option to keep the line style that same as the leader/dimension style with the option “Same as leader style”. If you wish to use the document defaults, selected “Use document display”.
If both of these settings are unchecked, you can set the extension line for the selected dimensions separately from the dimension line style. The example here shows the line thickness as different.
Second, you can now set individual extension lines to display as centerlines. This allow you to identify extension lines that emanate from holes, per ASME practices. To make this change, right-click on the extension line and select “Set Extension Line as Centerline”.
To change it back to normal style, right-click on the extension line again and select “Reset Extension Line Style”.
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
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)
This information was previously posted as part of another article, to which Vajrang Parvate (SolidWorks Corp Sr. Manager, Drawings Development) replied with an additional helpful hint. I’m reposting as a separate article to highlight the information.
Deleting Dimensions behavior
SolidWorks has a new user-selectable behavior when a dimension is deleted. If the user deletes a dimension or even just removes text from a dimension, SolidWorks has the ability to automatically realign the spacing of the neighboring dimensions to get rid of gaps caused by that deletion. The user has the option to turn this ability on by going to Tools>Options…>Document Properties>Dimensions to select the Adjust spacing when dimensions are deleted or text is removed checkbox.
Undoing the deletion
…When the “Adjust spacing when dimensions” checkbox is checked and SolidWorks moves in dimensions after one is deleted, two commands are added to the undo stack : one for the deletion of the dimension and another for the movement of the rest of the dimensions. So hitting Ctrl-Z will undo the deletion in two steps.
One of the funny little things that SolidWorks used to do is that when one added a center mark to a hole (or set of holes) that are already dimensioned, it would not adjust the dimension extension lines to fit with the center mark.
In the march to quality improvements, SolidWorks has fixed this little oversight. Now, when one adds a center mark to a previously dimensioned hole, a gap appears between the center mark and the dimension’s extension line. The same is also true if one adds a dimension to a hole that already has a center mark. No more dragging extension lines after the fact.
Here’s the sample image from the What’s New file:
Adding dimensions to parts on drawings is now quicker in SolidWorks 2010 with the addition of Rapid Dimension. Once the user enters the Dimension command, Rapid Dimension allows the them to quickly position dimensions (almost automatically) as they are added. Not only will dimensions automatically space out correctly as they are inserted, they will be inserted at the correct location, even without that location in view.
Now, each time a dimension is added to a drawing, SolidWorks will pop up with a pie, divided into two pieces for linear dimensions or four pieces for radial dimensions. (Technically, these pies are called the rapid dimension manipulators.)
Each piece of the pie represents the direction (which side of the part) that the user can choose to place their new dimension. When the user selects the half or quarter, the dimension is placed in the correct location on that side of the part within the drawing view.
Two methods can be used to select the dimension location using the pie. The user can simply LMB click on the portion of the pie in the desired direction. The user can also use a mouseless method, by pressing tab to toggle between the pieces of the pie; then press the spacebar to select. Additionally, the user can choose the ignore the choices offered by the pie to manually place the dimension, just as they would in previous versions of SolidWorks.
The auto-spacing between dimensions is determined by the user’s settings in Tools>Options…>Document Properties>Dimensions within the Offset distances field. The ability to set default dimension line offsets has been in SolidWorks for quite some time, but it’s never been quite so useful as it is in Solidworks 2010.
Within a few minutes of using Rapid Dimensions, many users will likely become instantly addicted to the new function, as it promises to be a major time saver when detailing drawings in SolidWorks 2010 and beyond.
One additional item about dimension placement is SolidWorks behavior when a dimension is deleted. If the user deletes a dimension or even just removes text from a dimension, SolidWorks has the ability to automatically realign the spacing of the neighboring dimensions to get rid of gaps caused by that deletion. The user has the option to turn this ability on by going to Tools>Options…>Document Properties>Dimensions to select the Adjust spacing when dimensions are deleted or text is removed checkbox.