What’s New in SolidWorks 2013: Section View Assist Part 2 – Shortcutting cutting line creation

This entry is part 11 of 12 in the series New in SolidWorks 2013

Auto-start section viewSection View Assist automatically comes up when you start the Section View tool without preselecting a sketch.  Section View Assist allows you to create very complex section views very quickly.  It also allows you to make the simplist section views faster than before, without the need to draw sketches on your drawing view.   Included in the new tool is the ability to shortcut the creation of simple section views even more!

If you do not use more complex section view cutting lines very often, you can by-pass the Section View Pop-up by checking the “Auto-start section view” setting.  This will allow you to place the cutting line and then immediately place your section view.  The setting is sticky, so you wouldn’t need to choose it again.   If many cases, you can create your section views with just two quick mouse clicks.

 Select Geometry   Place the view


What’s New in SolidWorks 2013: Section View Assist – Part 1

This entry is part 10 of 12 in the series New in SolidWorks 2013

SolidWorks 2012 and prior had two separate tools to create section views in drawings, Section View and Aligned Section View.  Although these were very capable tools, there was two different workflows to create cutting lines for section views based on which tool was chosen.  The two types of section views where not interchangeable.  Both used sketches to determine the path of the section view cutting line.   However, both tools produced very different results with the same sketch layout.

Section View tool changeSolidWorks 2013 unifies these separate types of section views, along with half section views, into one tool called Section View.  This new tool has expanded capabilities, being able to handle a wider range of section view types and scenarios.  For example, you can now add arc offsets to your cutting line and get the correct display in the resulting section view.  There are many other improvements as well.

When the new Section View tool is launched (without preselecting a sketch), a new user interface appears, called Section View Assist.  Section View Assist allows you to rapidly generate cutting lines for your section views without needing to draw sketch entities.  Four options for standard section views are immediately available: Vertical, Horizonal, Auxiliary and Aligned.  Each of these can be  previewed on any standard drawing view.  Use Tab and Shift-Tab to cycle through the preview choices.  Relations to geometry are automatically identified during the preview.

Vertical cutting line:

Vertical cutting line

Horizontal cutting line:

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Auxiliary cutting line:

5-9-2013 8-42-42 PM

Aligned (bent) cutting line:

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To accept the cutting line placement and geometry relations, simply LMB click when the preview is at the desired location (more clicks will be required to place Auxiliary and Aligned cutting lines).  The Section View Assist will then set the preview of the cutting line on the drawing view with any applicable geometry relations.  Additionally, the Section View Pop-up appears nearby.

Cutting line preview is placed and turns black

To accept the cutting line location, RMB click OK or select OK button from the Section View Pop-up.  Then, just place the section view on the drawing sheet.  In many cases, you can add you section view as easy as 1 – 2 – 3 clicks without the need to draw sketches.

 Section View created

Note: you can still create a sketch and preselect it prior to starting the Section View tool.  This will allow you to bypass Section View Assist and use the same workflow as in SolidWorks 2012 to create a section view.

What’s New in SolidWorks 2013: New capabilities of Exploded Views

This entry is part 9 of 12 in the series New in SolidWorks 2013

Multiple exploded views per configuration

In assemblies and multibody parts, the ability to create multiple exploded views for each configuration is now available.  As before, each exploded view appears under the specific configuration in the Feature Tree at the Configurations tab.  Now, multiple exploded views can appear as a list under each configuration .  This means you now longer need that the old workflow of having to maintain separate configurations for separate exploded views, even when the configurations are otherwise identical.

This functionality is also now supported in eDrawings.

Copying exploded views

Additional power has been added to exploded views and configurations where you can use normal windows Copy-and-Paste functions (CTRL-C/CTRL-V) to copy and paste exploded views between configurations!  To do this, highlight an exploded view in one configuration and hit CTRL-C.  Go to another configuration in the same assembly, and hit CTRL-V. Easy!

What’s New in SolidWorks 2013: Intersect (Wow!)

This entry is part 8 of 12 in the series New in SolidWorks 2013

SolidWorks 2013 introduces a new and powerful tool called Intersect. Intersect enables you to perform complex operations to quickly combine surfaces, planes and solid bodies in practically any way you need without the need for multiple cut, trim and fill features.  The tool’s visual interface allows you to do all the experimenting you’ll need in order to create the final shape you want.  The following is an example of how Intersect can help you to quickly build a part from multiple intersecting surfaces.

This is a set of surface bodies that will be used to create the exterior of a new consumer product.  The goal is quickly combine these surface bodies into a final solid shape that can then be shelled.

Series of surface bodies

  1. Intersect PropertyManagerStart the Intersect tool (found on the Features toolbar).
  2. Select all of the surface bodies.  As you select each one, they populate the Selections box in the PropertyManager.  Hint: you can use window select to get all the surface bodies at once.
  3. Choose Intersect button.
  4. A list of intersection regions is quickly generated in the Regions to Exclude box in the PropertyManager.  In the case of this project, there is only one region, so there will be nothing to exclude.
  5. Make sure Merge result is checked on the Options box in the PropertyManager.
  6. Because we do not want the surface bodies to remain in the final part, make sure Consume surfaces is also checked.
  7. Once you are satisfied with the previewed result, choose OK (green check mark button) to accept and apply.
  8. The result is finalized.  The entire operation appears as one new Intersect feature in the Feature Tree.
  9. Adjustments to your selections can be made at any time by editing the Intersect feature in the same manner as any other features are edited.

Preview of result

Preview of result
Final result
 Final result

Sometimes it’s the little new things (~part II) in SolidWorks 2013: Watermarking

This entry is part 7 of 12 in the series New in SolidWorks 2013

There’s been a long trail of discussions on the topic of adding watermarks to SolidWorks drawings.   For one reason or another, watermarks are seen by some as necessary in drawings.  The starting point of the conversion can be roughly traced back to the SolidWorks Forum in 2006.   In December 2007, I did one article that incompletely addressed the need.  If you just needed text to show up on your sheet format, you can review the first article.

Then, a question was asked at the first Stump the Chumps presentation at SolidWorks World 2008 about how to add watermarks to drawings.  No answer was given at that presentation (the chumps where stumped).

Soon after SolidWorks World 2008, Ben Eadie (one of the stumped chumps) found an About SolidWorks article that discussed various aspects of this topic.  (The article appears to have been maintained/updated since then.)     Around that time, I also wrote a detailed article about how to link your custom properties to your watermark and provided a trick  to get the watermark note to appear underneath elements on the drawing sheet.  Linking custom properties to the watermark allows the watermark value to be controlled by Enterprise PDM workflows.

OK, so what was the trick to getting notes to appear underneath drawing elements? If you created a block of an annotation note on your sheet format, that note block will appear under your drawing (without obscuring drawing content).

In Solidworks 2013, you no longer need to use that trick to get your sheet format note to appear underneath drawing elements.  There is now a command that resides in the right-click menu for each annotation note on the sheet format called “Display Note Behind Sheet”.  When checked, the  note is placed underneath drawing view elements on the drawing sheet, including other annotations, dimensions and model geometry in both HLR/HLV and shaded modes.

Display Note Behind Sheet is a checkmarked command in the
right-click menu for any annotation note on the sheet format.

With the checkmark set on the note in sheet format, the
note appears under all drawing view elements.
Uncheckmarking the option will apply standard ordering
of drawing elements, with geometry obsured by
the note.