Year of the Angle Dimension – Part 5 – Take a 180

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

What do you do when you need to create an angle dimension at 180 degrees? Maybe you need a 180 degree angle driving dimension between two sketch lines for sketch mechanisms. Maybe you just want to show the relationship between two parts of an assembly at a particularly point in their motion relative to each other, expressed as configurations. Or, maybe you just want to create a 180 degree angle, just because. Previously, you were blocked from creating such a dimension directly. In order to create a 180 degree dimension, you had to move some geometry (sketch line, components, features) slightly off 180 degrees, create your dimension, then edit whatever was necessary in order to restore the 180 degree angle.

SOLIDWORKS 2015 Smart Dimension tool now supports the creation 180 degree dimensions directly. No longer is it necessary to use the workaround. For sketches, the two lines that form the rays of the 180 degree angle must either share a vertex, or be separated where a vertex is inferred from their intersection.  Just start the Smart Dimesnion tool and select two colinear non-overlapping entities, and a 180 degree angle will be generated for you.

180 DEGREES

 

Year of the Angle Dimension (Part 4): Symmetricality

This entry is part 4 of 5 in the series SOLIDWORKS 2015 - Year of the Angle Dimension

Previous releases of SOLIDWORKS introduced linear dimensions in sketches that can be applied symmetrically when created across a centerline.   Further enhancements saw smarter behavior, where the selected centerline is remembered for multiple dimensions created in sequence.  For SOLIDWORKS 2015, you can create multiple half and full symmetric angular dimensions without selecting the centerline each time.


Angle with centerlineTo create a symmetrical angle dimension
:

  1. In a sketch with a centerline and lines or points, click Smart Dimension at Tools>Dimensions>Smart.
  2. Select the centerline and another line which is at an angle to that centerline.
  3. To create a half angle dimension, move the mouse cursor to the desired location and click to place, as previously.  However, to create a full angle dimension (across the centerline), hold down the SHIFT key.
  4. Drag the mouse cursor (along with the previewed dimension) to the opposite side of the centerline.  As you do so, a preview of the angle dimension will appear symmetrically about the centerline.
  5. Click to place dimension as desired.
  6. Keep holding down the SHIFT key and select other lines at angles to the centerline.  Angle dimensions to the centerline will automatically generate and will allow you make more symmetric angle dimensions successively.

Year of the Angle Dimension – Part 3 – Goodbye Zero

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

When you use angles that are set to deg/min and deg/min/sec, there are often times when you’ll have zero (0) for one of the levels of units.  For example, an angle may be 43 degrees, 0 minutes and 20 seconds.  This is displayed as 43° 0′ 20″.  For many people, the 0 minutes is redundent and unnecessary.  SOLIDWORKS 2015 now has an option that allows you to show only the unit levels that have a non-zero value.  For this example, the display is 43° 20″.  This new setting can found at Tools>Options>Document Properties>Dimensions/Angle, and named “Remove units with 0 value for deg/min and deg/min/sec”.

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.

  1. Start the Smart Dimension tool.
  2. In a drawing view, select a model edge.
    Select edge
  3. Select a collinear and adjacent point (vertex or sketch point).Select vertex
  4. A crosshair appears over the selected point.  Select one of the crosshair’s segments.
    Select crosshair segment
  5. A preview of the angle dimension appears.
    Preview of angle dim
  6. Click to place the dimension.
    New Angle Dimension type

 

New in SolidWorks 2014 (not mentioned in the What’s New): View rotation angles everywhere (Part 3)

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

With all the new functionality with view labels in SolidWorks 2014, some ancillary enhancements have also come about as a result from customer feedback during Beta Testing.  One of these enhancements has been the new capability to display any view’s angle within an annotation note.  Why would anyone need something like this?

Well, there are four default options for the display of the angle symbol auxiliary views.

  • Show rotation symbol with rotation angle
  • Show rotation angle
  • Show the text “ROTATION” followed by the rotation angle and direction
  • Show just the angle

If your company chooses to display just the rotation angle (as is common for GOST drawings), it is still sometimes necessary to display the rotation angle.  Because the view label is a global setting within the drawing, there’s no way to accomodate this deviation from the standard settings without having some hugely complicated user interface to track individual labels here and there.  So, instead, one additional annotation tag has been added.  The advantage is that this new tag is available for any drawing view (not just auxiliary and section views).  The new tag is <VIEWANGLE>.  Type this into any annotation note.  As long as that note is a attached to a view, that view’s angle will be shown.  As an example, this new tag can be added to the auxiliary view label after the <VLANGLE> tag (or anywhere else in the note).

View rotation angle in any annotation note

The settings and the result of using the new tag:

Adding the tag to add back the angle

Rotating a Drawing View

Sometimes one need to show a rotated view in the drawing. If is available in the standard view, once can simply place it as desired. If there is no view as required, one may go to part or assembly and create a new view orientation and then use that in the drawing. To avoid that one can simply rotate the drawing view as required.

1. Click on the view or select the view you want to rotate.

2. Click on Rotate View on the heads up tool bar or standard tool bar.

3. You’ll now see a Rotate Drawing View pop up window.

4. Fill in the desired angle value (I have used 90°). You can also key in a negative value.

5. Once you have keyed in the desired value, click on Apply and view will be rotated.

6. Then click on close to exit the command and you’ll have a rotated view.