Tag: feature

External Threads in SolidWorks (where are they?)

One of the unexpected weaknesses in SolidWorks is that there is no External Thread feature.  For years, SolidWorks has had the Hole Wizard and related functionality for various types of holes, including threads.  But there is [was] no feature for creating external threads.  I’ve always been baffled by this.

[All this has changed as of SOLIDWORKS 2022 with the release of the new Stud Wizard tool!  The remainder of this article will be about my impressions before Stud Wizard tool from the original publish date.  I will italicize outdated statements below.  A new article will be posted at some point to review the new tool.]

Examples of Stud Wizard
From SOLIDWORKS 2022 Help File

So, when I saw that SolidWorks 2010 was improving the Cosmetic Thread annotation to allow the user to quickly choose a thread size from one of the thread standards (ANSI, ISO, etc), I had a brief glimmer of hope.  I found out, this is one of those enhancements that is just too little, too late.  All this new enhancement does is pull values from the Hole Wizard to add a Cosmetic Thread annotation.  If an external thread is desired, the user is still left with having to create the OD of the thread as a separate feature.

Sure, one may not expect an annotation to make a feature.  It just seems like an opportunity was missed.  Instead of just having the Cosmetic Thread annotation read from the standards, SolidWorks should have included an External Thread feature.

In my view, this feature should work in several ways.

  1. Allow the user to select an OD upon which the External Thread will be cut.
  2. Or, allow the user to select a flat face from which the External Thread will extend.
  3. Don’t require a precondition.  Allow the user to select their method within the workflow of External Thread command.
  4. Have the External Thread feature work the same way as Hole Wizard.  The helix of the thread is not modelled, but have several modelling and annotation options available (model to the ID or OD, and choice to use cosmetic thread).

Although the addition of the standards lookup within the Cosmetic Thread annotation is welcome, SolidWorks should fully support External Threads as an actual feature.  I created an ER for this topic this week, and invite others to do so as well.

[To see information about the new Stud Wizard (that works pretty much as I laid out above), see the What’s New for SOLIDWORKS 2022.  For more information, you can check out the SOLIDWORKS 2022 Help File articles about Stud Wizard.]

Control Root Size of Drafted Rib on Curved Surface

*This article makes some inaccurate statements regarding the capability of SolidWorks.  Please see the correction article for details.  Inaccurate statements have been crossed out.  The methodology described in this article should be referenced as an example of bad practice that should only be employed if traditional methods fail.  Edits to this article appear in this color.*
*Additional comment: this article does demonstration a good method for getting a line along a curved surface into a sketch. *

Good mold design means that one must take care to control the root width of a rib.  How does one do this if the rib is based on a curved (non-prismatic) surface? 

SolidWorks has many powerful features for making injection molding parts.  It has both rib and draft features.  Unfortunately, these two features together have one important limitation.  When applying a draft to a rib based on a curved surface, SolidWorks does not allow the user to hold the root width of that rib.  SolidWorks requires a prismatic surface to use as a neutral plane from which to start a draft.  This means in this case, the draft can only be started from the top of the rib, not its root.  If one wishes to hold the rib root constant along a curved surface, one cannot use the rib or the draft features.

SolidWorks does have an arsenal of other features and tools to allow one to build an alternative strategy to workaround this limitation.  

Basic shelled part with curved surface

This first figure shows a fairly simply shelled injection molded part with a complex curved surface.  To make drafted ribs using this method, first create an axis that can be used as an directional guide. You can choose to use features on the part itself for this purpose, instead. I prefer to create a special sketch at the location where I plan to add a boss.  Regardless of the method used, the directional guide should be parallel to the direction planned for the ribs.

 Setup Sketch for Directional Guide

The second step is to start a new sketch above the curved surface.  In that sketch, draw the outline of the rib.

Sketch outline of ribs

If there is a series of ribs needed in one direction, try creating a sketch pattern the other instances.  Make sure to turn sketch entities of the other instances into construction lines.

Project outline using Split Line

Use Split Line to project that outline onto the curved surface.  Split Line will only project one contour per sketch.  This is why it is important to turn all other instances of the rib into construction lines.  Having those other instances pre-drawn will save time when making the other ribs (covered in Part 2 of this article). 

Next, start a 3DSketch.  Use Convert Entitles to bring the Split Line curves into the sketch.  Drag the end points of the curves so they are coincident (on the surface) of the outside surface of the outer walls, or some othe appropriate location.  Then, close the contour by drawing lines to connect the curves at each end. 

Convert split line edges in 3DSketch

Extrude this sketch.  Use the previously drawn axis from the first sketch as the direction.  Use the top surface of the cavity (or whatever is appropriate) as up-to-surface entity.  Turn on Draft and specify the desired angle.  Here’s the funny part.  Be sure to extrude a small amount (smaller than the wall thickness of the part) in the other direction without draft.   If this isn’t done, a zero-point error will pop up preventing the completion of this step.

Use previous setup to set extrude of 3DSketch

The end result will be a drafted rib with a controlled root width.

Final result

Part 2 of this article will detail how to create repeated and crossing ribs using this same technique.  Again, please note this is not a best practice method.  See the correction article for details.