Correction on Rib/Draft on Curved Surface Article

I stand corrected on a previous article.  I originally made a misstatement regarding the capabilities of SolidWorks to create drafts on ribs based on curved surfaces with controlled root widths.  As far as an explanation for this oversight, I can only say what didn’t work for me last week worked this week, and that my VAR has some new inexperienced people on their phone support.  Here’s the basics that didn’t work before but work today.

SolidWorks does allow one to control the root width of a rib feature on a curved surface with the draft feature.  This means that draft will diminish from the ribs base, even if it is from a curved surface.  To apply a draft to such a rib, simply use the parting line option and pick a perpendicular plane or a parallel line/entity for the direction of draft.  For the parting line, choose each of the edges where the rib intersects its curved surface base.  If necessary, toggle the direction of draft.  That’s it. 

Of course, this method is still imperfect.  The question is, why doesn’t the draft feature just know that I want to pull it from the root?  It seems illogical to require a neutral plane at all since each rib has only two ends.  Why not just ask the user for the end to draft from?  I guess if someone wants to use draft to add angle to a rib long its left to right/up to down, then making this assumption wouldn’t work.  I doubt that would be much of an issue however, since that is not what a rib nor a draft is supposed to be.

The alternative method I posted last weekend should be referenced as a case of bad practice that works and should only be used if nothing else does.  Edit: however, it is a good demonstration of how to get a line along a curved surface into a sketch.

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.