Pointy arrows without the ears (a.k.a, text)?

Every once in awhile in drafting, you just need an arrow, with no text, attachments or any other extras.  Maybe you need to specify air flow, grain direction, inspection queue, assembly instructions, or one of a hundred other reasons.  How do you make just an arrow in SolidWorks?  Answer: Multi-jog Leader annotation tool.

Mutli-jog Leader is an oft overlooked tool that pretty much lets you make whatever arrow configuration you like using the same leader style of notes. 

To make a simple leader with no text, start the Multi-jog Leader and select your first point.  One arrow will point to the location where you clicked.  The other end of the leader will follow the mouse cursor.  Choose a second location and double-click to complete your leader.  This will add another arrow directly opposite your first arrow.

Get rid of one of the arrows by RMB clicking on the tip of the undesired arrow and choosing the arrowless option.


Here’s what you end up with. 

You can adjust the other end to be bigger (by RMB clicking on it and selecting Size…). In the case of the example below, I’m using the arrow to represent fluid direction of a flow body.

Recently found in the SolidWorks Blogospere

There is a number of good articles that have popped up recently in the SolidWorks blogospere.  Here is a selected set of particularly interesting finds:


How to add a Geometric Tolerance frame to your Sheet Format

**OUTDATED Content: Update–>SOLIDWORKS 2020 now allows you to add Geometric Tolerance and Surface Finish symbols onto your Sheet Formats directly without the following workaround**

SolidWorks Sheet Formats do not support Geometric Tolerance frames.  So, what can be done if you wish to display a frame with your Sheet Format on drawings?

First, a quick review.  SolidWorks has two separate files that serve as the starting point for creating new drawings.  The primary file is the Drawing Template (*.slddot).  Every time you start a new drawing, it must be from an existing Drawing Template.  The template contains all the settings and other information needed for every drawing.  In particular, it uses information from a Sheet Format (*.slddrt) for the border and title block.  Each time you create a new sheet on your drawing, the Sheet Format is directly loaded.  However, neither the Sheet Format or the Drawing Template automatically update existing drawings.  For more information on Sheet Formats and Drawing Templates, see SolidWorks Help.  The tip found in this article is for more advanced users and CAD Administrators that are already familiar with these topics.

Back to the story.  Perhaps your company is moving towards using the model to define your product, but still uses the drawing to established specifications, such as tolerances, general notes, process control dimensions, etc.  Common practice for this scenario is to establish a generic Profile specification on the drawing that is then applied to the model.   But, you cannot store a Geometric Tolerance frame within a Sheet Format.  You won’t likely want to draw your frame using sketches.

Solution? You can have a Sheet Format display a Geometric Tolerance frame that is present on a Drawing Template!  Here’s how.

1.  First, make backup copies of your Sheet Formats and Drawing Templates!  OK, once that is done, open your Drawing Template using File>Open dialog set to Template (*.prtdot; *.asmdot; *.drwdot)

2. Create your Geometric Tolerance frame using the Geometric Tolerance annotation tool.

3. Place your new frame in the lower right corner of your Drawing Template.  Don’t be concerned if it overlaps the border, but it is a good idea to keep it inside the paper space.

4. Create an annotation note (Insert>Annotations>Note…) and place it anywhere on the drawing.

5. While the annotation note is still being edited, click on the Geometric Tolerance frame.  The frame will now appear in the note.  Select OK to accept.

6. Select the new note.

7. Press CTRL-X.  The note should disappear, as it is being cut from the Drawing Template.

8. RMB click on any empty area of the blank paper space and select Edit Sheet Format.  This will take you into the Sheet Format editing mode.

9. Click on the approximate location where you wish the frame to appear and press CTRL-V.  This will insert the note onto the Sheet Format.  Click and drag it to the desired location.

10. RMB click on an empty area of the paper space.  Select Edit Sheet.  This will exit the Sheet Format mode and return you to normal drawing mode.

11. RMB click on the original Geometric Tolerance frame and select Hide.


12. Goto File>Save to save your Drawing Template.

13. Goto File>Save Sheet Format to save your Sheet Format.

(14.) Now, if you wish to edit the frame later, simply use View>Hide/Show Annotations.  The hidden frame will appear faded gray.  Select it and it will turn black.  Press ESC to exit the Hide/Show mode.  Edit the frame as your normally would any Geometric Tolerance frame.  When done, hide it again.  You may need to Rebuild to see the update.

Note:  If you open the Sheet Format directly without loading the Drawing Template or if you load the Sheet Format into a drawing created with an older Template, the annotation note containing the frame will be blank.  This is because the information is contained in your new Drawing Template, but the note is in the Sheet Format.

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.

Auxiliary views for those strange angles

I rarely used auxiliary views.  Every once in awhile, parts defy orthogonal projection.  These are when auxiliary views are useful.  In those cases, auxiliary views are generally projected from some perpendicular surface.  But once in awhile, there’s a part that defies even this, having no flat surfaces from which to project.  

In the example below, there is a feature that cuts through a part at an odd angle.  There is no flat surface into which it cuts.  Normally, in SolidWorks, the direct view of this cut could be shown by using the Auxiliary View tool and selecting a perpendicular surface from which a view may be projected.  Here, there is no such flat surface.  SolidWorks does support these kind of oddball scenarios.  

In this example, we are still going to make use of the Auxiliary View tool.

1. Add a side view of the part.

2. Sketch a line onto the view. 

3. Add relations to the sketch line to make it perpendicular to the feature that is to be detailed.


4. Pre-select the line and then chose the Auxiliary View tool from the Drawing toolbar or at Insert pulldown menu>Drawing View>Auxiliary. 

5. A preview will appear attached to the mouse cursor.  Move the cursor in the direction that will be projected and click to place the view.  Depending on the version of SolidWorks, some further adjustment may be necessary to show the view arrow and other details with certain perferences.

Match up projected Break View with its parent view

Break views are common practice for some industries where long components do not fit well on standard sheet sizes at a useful scale.  SOLIDWORKS has a function to break views in the Break tool in the Drawing toolbar.  However, what if there is a projected view of that component that must also have a break?  Do the breaks in each view automatically track with each other (match up)?

Yup, but as with many abilities in SOLIDWORKS, there’s a setting.  This setting allows the user to determine if they want the projected view to always match up with the breaks in the parent view.  This choice is important, as there may be very real purpose to not have breaks in views line up.  For example, the parent and projected views may show details at different locations along the length of the component.

Unaligned break view


However, if the user wishes the parent and projected views to break at the same locations, the setting is located for the projected view in its PropertyManager>More Properties… button>Align Breaks with Parent check box.








End result in this example after a quick rebuilt (CTRL-B):

Break View UPDATE!

Newer versions of SOLIDWORKS automatically set Align breaks with parent property as checked. If you wish to have a projected view with different break alignment from its parent, you’ll have to uncheck this setting.