I know the SolidWorks Legion has been quite for a week or so. Worry not, we are still around. I’m personally working on 3 product reviews. Stay tuned!
Order of Business: Possibly Rename Resources Site
I am considering renaming Lorono’s SolidWorks Resources website. I’ve not made up my mind if I want to or should. So, let me ask others. What do you think of the name? Does it represent that website? Should I associate it more closely with SolidWorks Legion (Legion SolidWorks Resources; SolidWorks Legion SolidWorks Resources) or modify and enhance its identity in some other way? Do you have any thoughts about this? In fact, what are your thoughts about Lorono’s SolidWorks Resource website in general?
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 I originally made a misstatement regarding the capabilities of SolidWorks to create drafts on ribs based on curved surfaces with controlled root widths.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.Â
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.
Order of Business: New Members
First, I would like to welcome two new members to the SolidWorks Legion.
Roland Schwarz (aka TheTick) will be making an appearance from time to time as a guest author, though I’m not going to stop him from posting articles daily if he wishes. 🙂 However, he may be a little too busy for that since he has recently started his own blog Tick Talk on EsoxRepublic.com. His is a major contributor to forums such as eng-tips.com and SolidWorks Forum. I am elated to have him on board.
I also welcome Joseph Aisawa to the SolidWorks Legion. He brings with him a fresh perspective about SolidWorks and our community. I look forward to having him relate experiences from school and things he has discovered since. This may help newer SolidWorks users by letting them know they are not alone (or even what to expect once they are out of school), and help long-term users by giving them a window into how our field is developing from the perspective of the next generation.
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?Â
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. Â
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.
 
The second step is to start a new sketch above the curved surface. In that sketch, draw the outline of the rib.
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.
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).Â
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.Â
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.
The end result will be a drafted rib with a controlled root width.
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.
Dual Dimensioning and ASME Y14.5M-1994
Dual dimensioning is the drafting practice of using multiple units of measure in a dimension in the same direction of a feature. SolidWorks and many other CAD programs support dual dimensioning. This support is usually a little quirky. It’s actually not the fault of the CAD application. At one point, it was a surprize to me (and often is to others too) that no current drafting standard actually supports dual dimensioning. In retrospect, this makes perfect sense.
My experience is with ASME Y14.5M-1994. When invoking ASME Y14.5M-1994 (or even ANSI Y14.5M-1982), one will find that rules regarding dual dimensions do not exist. ANSI Y14.5M-1982 does mention in its appendix that support for dual dimension no longer exists in the standard. This is apparently because it was mentioned in a previous version. That said, dual dimensioning has never really ever been allowed by any incarnation of Y14.5. This is because of very specific wording under the standard’s Fundamental Rules. The wording may vary between versions, but carries the same meaning in all versions. In ASME Y14.5M, that wording is as such in 1.4(d), “Dimensions shall be selected and arranged to suit the function and mating relationship of a part and shall not be subject to more than one interpretation.” (Support for dual dimensions in pre-1982 versions was a mistake that was likely political in nature.)
General practice in the use of dual dimensions is that they are of equal importance to the primary dimension. This creates issues in that it allows for more than one interpretation of the dimension. It is nearly impossible for nominals and tolerance ranges to be identical between units of measure. This means that the dual dimension tolerance range is usually resized to fit within the tolerance range of the primary unit of measure. This creates a situation where the dimension has more than one interpretation, which is specifically prohibited by 1.4(d). The conclusion that can be drawn from this is that dual dimensions are actually not allowed by ASME Y14.5M-1994. This is the hard argument against the use of dual dimensions. I could end this article right here. However, I will also explore the soft arguments against their use.
ASME Y14.100-2004 paragraph 4.32.3 uses soft language to discourage the practice of converting inch to metric and vise verse (“should not be used”). This is known as soft conversion. This is not an outright prohibition against dual dimensioning by itself. However, the practice of soft conversion is integral to using dual dimensions. With this practice discouraged, dual dimensioning is also discouraged.
ASME Y14.5M-1994 defines a reference dimension as such,
“A dimension usually without tolerance, used for information purposes only. A reference dim is a repeat of a dimension or is derived from other values shown on the drawing or on related drawings. It is considered auxiliary information and does not govern production or inspection operations.”
By definition of reference dimensions, dual dimensions must be treated as reference dimensions. However, anyone who uses them knows this is generally not their intent. As generally intended, dual dimensions are disallowed unless they are considered reference only.
The final soft argument is gleamed in the wording of ASME Y14.5M-1994 paragraph 1.5. This paragraph assumes dual dimensions are not in use. For example it begins one paragraph as so, “Where some inch dimensions are shown on a millimeter-dimensioned drawing…”. It never then says “Where many inch dims are used on a metric drawing….” This is not a specific exclusion, but should be noted for its wording. It does allow for the use of both inch and metric units on the same drawing, but not multiple values of dimensions for the same features.
With all of these arguments aside, CAD applications do attempt to accommodate users who feel they need this capability. However, if used, caution must be exercised. Handling of dual dimensions by CAD (and common practice) can create confusion on a drawing, particularly if the software assumes values for the dual dimensions and its tolerances.
In the effort to avoid issues and violations of the standards, it is my opinion that if dual dimensions are used, they should be noted as for reference only on the drawing. This can be accomplished by adding a note similar to “DUAL DIMENSIONS IN BRACKETS ARE FOR REFERENCE ONLY.” This avoids problems caused by multiple interpretations for dimensions. Of course, over use of reference dimensions is also discouraged by ASME Y14.5M-1994. But hey, who’s it hurting?
For SolidWorks, dual dimensions on a drawing may be employed by going to Tools>Options>Document Properties>Detailing and checking Dual dimensions display. Also at that location is the choice to display the dual dimension on top, bottom, left or right of the primary dimension. These are SolidWorks 2007 instructions (other versions of SolidWorks should be similar).
I did make a sample SolidWorks macro that will turn on dual dimensions for a drawing and automatically set them to display on the bottom (default is top). This example macro can be downloaded here. It can be modified to use any settings as default.
For the record, this article was inspired by multiple posts on various SolidWorks related forums over the past few months such as these at SW Forums, eng-tips.com, and Pro/E discussion at eng-tips.com.