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:

Enjoy!

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**OUTDATED Content: Update–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.

GD&T Feature Control Frame user interface?

Remember this old faithful interface for creating Geometric Tolerance frames (a.k.a, GD&T feature control frames, or GTOL annotations)?

There a new thread on the Drawings forum at SolidWorks Forums asking about how you use this user interface to create Geometric Tolerance Frames.  Your input is very welcome there (and here, if you wish).  What would you do to improve the inferface?

  • When do you use it?
  • How does it work for you?
  • What do you think about the workflow of creating the frame before you place
    it on the sheet?
  • How do you feel about the preview window (and would it be necessary if you
    could just see your frame being modified directly on the sheet)?
  • Do the restrictions within the interface (meant to force you to follow
    GD&T rules) ever prevent you from creating the frame that you need?
  • Have you used the PropertyManager settings that also pop up when you edit an
    existing frame?

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.

eDrawings for iPad from 3DS SolidWorks ( #edrawingsforipad )

The much anticipated initial release of eDrawings for iPad is now available from the Apple App Store.  This is an inexpensive app ($1.99) to view SolidWorks models (.sldprt), assemblies (.sldasm) and drawings (.slddrw) on the iPad.  Of course, eDrawing formats (.edrw, .eprt, .easm) and .DWG are also supported.  All images in this article are actual screen shots.

Pages: Page 1, Page 2, Page 3

The official Photoview 360 book by SolidWorks ( @robrodriguez @solidworks )

Amazon Affiliate link to Photoview 360 guideAmazon Affiliate link to Photoview 360 guide
I’ve been wanting to write an article about the book Photorealistic Rendering Using SolidWorks and Photoview 360 for almost a year now.  Between that time and now, I’ve become employed by SolidWorks, which makes writing reviews about SolidWorks related products somewhat self-serving.  As such, I’m not going to do a full length detailed review.  That being said, it is a great guide to learn the ins-and-outs of making photorealistic images from SolidWorks.  One of the main consultants for this book is Rob Rodriguez, infamous for his photorendering skills.

The book’s approach to the subject is refreshing, in that it is written from the perspective of a photographer.  Topics include basic elements, such a lighting, to more complex visualization settings for illumination.  Also discussed are OpenGL, RealView, Surface Finishes, hardware, performance, scenes, decals, user interface, display states, configurations, mapping, output options, etc, etc.  It does include a DVD-ROM!

It’s a great guide with a lot of detailed images as it takes you step-by-step through the process of creating photorealistic images with SolidWorks and Photoview 360.

The book is available in the SolidWorks Store.  It is also now available from Amazon.com (image link above is via Amazon.com).