Category: Drawing

Visually determine the depth of a Broken-out Section in a Drawing View during preview

Adding a broken-out section to a drawing view is very useful to show detail inside of a part without resorting to creating an additional Section View.  The Broken-out Section tool in SolidWorks allows you to quickly add this detail to an existing drawing view by simply drawing a closed spline and establishing a depth.  A preview option allows you to see the result of your choices.  The drawing view updates in real time as you change depth.

However, sometimes, it is hard to visualize the depth while you are creating the broken-out section.  Some users will simply step through various depths until the broken-out section looks about right.  This trial and error method can be time consuming.

The Broken-Out Section tool is actually smarter than that!  It detects when there are projection views of the current view (either parent or child).  If there is a projection view, you can click on the specific feature you wish to slice with the broken-out section.  To use this cool function:

  1. With the Broken-Out Section tool active and cut area established, click on the Depth Reference field in the PropertyManager. 
  2. In the adjacent side view, you will see a yellow line that represents the current depth of the broken-out section cut.  Click on the feature you wish to cut through.  The depth line will shift to the center of that feature.
  3. Click OK to accept.

The above method may not always be feasible.  Perhaps the detailed components are too large to show the multiple views on screen at the same time.  Or, perhaps there is no feature that readily provides desireable results.

Here’s a trick that may help.  Use 3D Drawing View tool to rotate the view in 3D.  As you adjust the depth in the PropertyManager, the 3D view of the model will update accordingly.

1. With the target view highlighted, choose 3D Drawing View tool.

2. Rotate the view to a desirable angle.

3. In the PropertyManager, change the depth.

4. Select OK in the PropertyManager when desired depth is found.  Then exit the 3D Drawing View tool.

The result is a happy broken-out section in your target drawing view.

SolidWorks 2012: Reuse Letters from Deleted Views

In the past, SolidWorks would track the letters used in Section Views, Detail Views and Auxiliary Views on drawings. If one of these views was deleted, for whatever reason, it’s letter would no longer appear on the drawing when new views were created. The only automatic method to get the letters to be reused would be to reset the starting letter for the whole drawing. What many users ended up doing was just manually entering letters for new drawing views after one was deleted.

In SolidWorks 2012, a new setting was added that allows you to automatically reuse letters from views that have been deleted.  This setting is in Tools pulldown > Options… > System Options tab > Drawings heading.  Near the bottom, find Reuse view letter from deleted auxiliary, detail, and section views.  Add a check to its box and OK.  The setting’s name is a bit long, but clearly stated.

So, now when a view is deleted, it’s letter will automatically appear for the next Section View, Detail View or Auxiliary View.

 

Some New Macros to tangle with

Recently I posted some new SolidWorks macro at Lorono’s SolidWorks Resources which you would like to try and might find useful for your day to day use.

Here are brief details on the macros:

Send Email via SolidWorks : Macro to send email with assembly name in subject.

Save and Open as PDF:  Macro to save active file as PDF in the same location and open the created PDF file

Hide Show Note : Macro to hide or show note in the active drawing.

There are more useful macros and stuff at Lorono’s SolidWorks Resources and I’ll be adding more similar macro there, so keep watching.

Rulers!

Although the status bar of the SolidWorks drawing mode always displays the X and Y coordinates of the location of the mouse cursor on the drawing sheet, sometimes the visual aid of a sheet ruler may provide additional help. 

SolidWorks drawing mode rules can be turned on at View pulldown>Rulers.

Once turned on, the rulers appear at the top and left edges of the drawing window.

The rulers also enhance the usefulness and feedback when the Grid is displayed. This is because the rulers provide constant confirmation as to the mouse cursor’s drawing location on the screen, no manner how far in the zoom level.

This makes keeping track of one’s position on the drawing sheet more intuitive, especially during sketching and using snap-to-grip functionality.

Control over various aspects of snapping and grid are available in Tools pulldown>Options…>Document Properties>Grid/Snap. 

Changes to grid increments are reflected in the rulers.

New in SolidWorks 2012: Improved placement of Section View Labels (Another one not mentioned in “What’s New”! )

In previous versions of SolidWorks, when you attempted to move the Section View letter by clicking on it and dragging, very strong soft snaps would often force the location of the letter to fall into one of two set locations around the Section View cutting plane line arrow.  The snaps seemed even stronger if you were zoomed out a bit.

In SolidWorks 2012, users now have more intuitive control over the the placement of a Section View letter when they wish to move it.   The two snap locations are not nearly so strong.  It is still very easy to place a letter at one of the two locations by dragging and hovering the letter over the arrow tip or the bend in the cutting plane line.  However, it is also much easier if you want to place the letter at a different location; particularly when you are zoomed out.

This improved functionality will help users that like their Section View letters to appear at alternative locations for style or maybe because of a very busy drawing with limited space.

What’s new in SolidWorks 2012: Magnetic Lines

Just over a year ago, 3DVIA was showing off something called Magnetic Lines.  In 3DVIA, Magnetic Lines are a documentation aid that allows you to quickly line up any type of objects with each other by attaching them to a common line.  Most notibly, Magnetic Lines can be used to quickly align item balloons on assembly drawings.  Many users asked the question, if it is in 3DVIA, why not have it in SolidWorks.  Well, the SolidWorks team took the request seriously.  Within one year, they introduced Magnetic Lines in SolidWorks. 

Unlike 3DVIA, SolidWorks’ Magnetic Lines only control item balloons.  (SolidWorks has other tools to align annotation notes and drawing views.)  You can add a Magnetic Line to your drawing with the Magnetic Line command from Annotations toolbar or the Annotations tab in the CommandManager.

This will enable you to draw a line on your drawing with two points, thus forming a Magnetic Line.  You can drag one end of the Magnetic Line through the center of an existing balloon to attach it to the line.  You can also drag a balloon onto a Magnetic Line.  Magnetic Lines are only visible when the command is active, or when a  balloon is selected. 

Once balloons are attached, they can quickly aligned in any direction by dragging one end of the Magnetic Line.  They can also be moved in unison by dragging the Magnetic Line from the middle.

To detact a balloon from a Magnet Line, click on the balloon to drag it off of the line.  In my opinion, just about everything with this new tool is intuitive and easy!  It is a powerful new drawing aid that makes organizing balloons on assembly drawings much easier.