Category: Drawing

Drawings Top Ten list from years past: SWW2011

This entry is part 1 of 4 in the series Past Years Drawings Top Ten

Each year, SOLIDWORKS World has a top ten enhancement ideas countdown.  For a couple of months before SOLIDWORKS World, ideas are submitted by users to the SOLIDWORKS World Top Ten idea forum (login required). Starting in mid-December, users have the opportunity to vote on the ideas they most want.  This gives SOLIDWORKS a clear snapshot of what our customers need at that moment in time.  The top ten vote-getters are shown on the big stage at that SOLIDWORKS World. The list varies from year to year as new enhancements are implemented or as customers’ needs change. Some ideas also reappear on the list over several years.

Dan Herzberg has compiled a list of these top ten lists, including when the ideas where implemented and how many times an idea appeared on the subsequent lists.

There is no focus on particular areas in the top ten list. The top ten highest vote-getting ideas are combined from parts, drawings, assemblies, and other areas.   Since my main focus area on the SOLIDWORKS brand is “drawings”, it seemed like a nice idea to show the results for just the submissions for drawings.

We can show just the top ten Drawings ideas.  Drawings includes topics such as BOMs, annotations, dimensions, etc. The first year we can look at is SolidWorks World 2011.

SolidWorks World 2011 Top Ten Drawings Ideas

  1. Ability to Filter BOMs
  2. Print Selection – make it more like cropping a picture
  3. On drawings: add function to allow users to apply capitalization of text, implemented in SW2013
  4. Assign watermark function to drawing sheets, implemented in SW2013
  5. Allow Multiple Exploded Views per Configuration, implemented in SW2013
  6. More control over angle dimensions, implemented in SW2015
  7. On drawings: Allow option for resizing of drawing view outline
  8. Directly editing notes with properties in Drawing, implemented before SW2013
  9. Broken-out Section in Section, Detail and Alternate Positions Views
  10. Better line selection in drawings, implemented in SW2014

The implementation rate for the SWW11 drawing list is 60% to date.  None of these ideas had enough votes to get onto the official SolidWorks World 2011 Top Ten list, unfortunately.

There is still a couple of days to add new ideas on the current SOLIDWORKS World 2015 Top Ten list.  Voting starts on the 15th, so go back and vote on as many ideas as you wish!  Just remember, you have to logon to submit, see and vote for ideas.

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 [part not set] 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 2 – Flipping out (and over)

This entry is part 2 of 5 in the series SOLIDWORKS 2015 - Year of the Angle Dimension

In SOLIDWORKS 2015, there are two methods to change (flip) an angle dimension.

Vertically Opposite Angle

You can now flip any placed angle dimension to its vertically opposite angle.   This is useful when you wish to place the entire angle dimension outside of the model edges.

  1. Right-click on the angle to bring up the right-click menu.
  2. Select Display Options, then Vertically Opposite Angle.

Original angle dimension   Vertically Opposite Angle

Explementary Angle

You can now flip any placed angle dimension to its explementary angle.  Here is a way overly complex video about explementary angles.  Here’s a simpler explanation straight from the dictionary.

  1. Right-click on the angle to bring up the right-click menu.
  2. Select Display Options, then Explementary Angle.

Original angle dimension   Explementary Angle

Choose Explementary or Vertically Opposite in dimension preview

When creating an angle dimension with Smart Dimension tool, you can now choose between the explementary angle or the vertically opposite angle during the preview by holding down the ALT key when the mouse is in the vertically opposite region.  In SOLIDWORKS 2014 and prior, you were only offered the explementary angle.