dimension Archives - Page 2 of 4

Year of the Angle Dimension – Part 1 – Imaginary Rays

This entry is part 1 of 5 in the series SOLIDWORKS 2015 - Year of the Angle Dimension

There was a heavy focus on expanding functionality of angle dimensions using the Smart Dimension tool in SOLIDWORKS 2015. These enhancements streamline drawing detailing and sketch creation tasks. Here’s the first of such enhancements.

There is a long standing request for the ability to apply angle dimensions where one ray is aligned to geometry (model edge or sketch line) and the other ray is along an imaginary vertical or horizontal direction. In SOLIDWORKS 2015, there is a new capability with Smart Dimension tool that enables you to create this type of angle dimension.

Start the Smart Dimension tool.
In a drawing view, select a model edge.
Select a collinear and adjacent point (vertex or sketch point).
A crosshair appears over the selected point. Select one of the crosshair’s segments.
A preview of the angle dimension appears.
Click to place the dimension.

New in SolidWorks 2014: Dimension display controls

This entry is part 8 of 13 in the series New in SOLIDWORKS 2014

Extension and dimension lines 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.

Example

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”.

Set extension line as centerline

Centerline

To change it back to normal style, right-click on the extension line again and select “Reset Extension Line Style”.

New in SolidWorks 2014: Angular Running Dimensions

This entry is part 5 of 13 in the series New in SOLIDWORKS 2014

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.

Horizontal text

Aligned text w/ chain

Inline text w/ chain

Horizontal text w/ chain and bidirectionality

What’s New in SolidWorks 2014: On-The-Fly Virtual Sharps While Dimensioning

This entry is part 3 of 13 in the series New in SOLIDWORKS 2014

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)

Point Location (Virtual Sharp)

Point Locations by another name, such VIrtual Sharps

The names for dimensioning methods within ASME Y14.5 often do not match the common names. For example, what most of us call ordinate dimensioning is officially labelled as rectangular coordinate dimensioning. This can make information about certain dimensioning methods hard to find within the standard. One dimensioning method that is particularly difficult to find is point location. A point location is where a point is located by the intersection of extension lines only. The method is known by so many other names.

theoretical sharp corner
theoretical corner
theoretical sharp
apex
intersect
intersection
intersection point
imaginary point
virtual sharp
and likely others as well

The SOLIDWORKS application uses the term virtual sharp. SOLIDWORKS offers a list of options for the delineation of virtual sharps (i.e., point locations). These options are found at Tools pulldown>Options...>Document Properties tab>Dimensions heading>Virtual Sharps subheading. The only method supported by ASME Y14.5-2018 is the use of intersecting extension lines from two surfaces; so called witness in SOLIDWORKS.

The standard does not require any other identifier or labelling. Yet many of us do feel compelled to add some sort of label to the dimension, using one of the above terms or their initials. A label does add clarity, particularly when the scale of a view makes display of a point location hard to read.

I covered this topic once before from a slightly different perspective in this article: Virtual Sharps. That article includes instructions on how to create a virtual sharp in SOLIDWORKS drawings.

SolidWorks 2010 Deleting Dimensions

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

From Parvate:

…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.