Page 297 - Mastering SolidWorks

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Selecting a SPecialty Feature 269

the standard planes moving with respect to the rest of the part as little as possible. If you needed
to scale about a specific point on the geometry, you would need to create a custom coordinate
system at that point and use that as the reference.
The Scale Factor works like a multiplier, so if you want to double the length, you would enter
the Scale Factor 2. This does not work like the Scale function in the Cavity feature, which is less
commonly used. Scale within Cavity uses a scale factor that is shown as a percentage increase, so
to double the linear dimensions of a part would require a scale factor of 100 percent. The Cavity
feature is available only in the context of an assembly and has fallen out of favor with most mold
designers.
Scale is also configurable, meaning that different configurations can use different scale factors.
Configurations are covered in Chapter 11, “Working with Part Configurations.”
An interesting aspect of the Scale feature is that you can disable the Uniform Scaling option.
This allows you to apply separate scale factors for the X, Y, and Z directions. In mold making,
this can be used if you have a fiber-filled material and the mold requires differential shrink
compensation based on the direction of plastic flow, and thus of fiber alignment (the part will
shrink less in the direction of fiber alignment). But you could also use it to size any general part.
Just remember that if you apply differential scale, circles may be distorted. To get around this,
you may be able to reorder the features to apply the Scale feature before the circular features
are added.
Because Scale is simply applied to the body rather than to features and sketches, it can be
applied to imported parts as well as SolidWorks native parts. Sometimes, people use the Scale
feature to compensate for improper imported units. For example, if a part was originally built
in inches and translated in millimeters, you might want to scale the part by a factor of 25.4.
You can also enter an expression in the Scale Factor box so that if the import units error went
the other way, you could scale a part down by 1/25.4. The limitation to the Scale feature is
that the SolidWorks modeling space for a single part is a box that’s approximately 500 to 700
meters centered about the origin. There appears to be some difference between sketching limits
and 3D solid limits.
An implication of the Scale feature that is not stated outright is that it does not scale features,
sketches, or dimensions. It is a history-based feature, so the size difference only applies after the
Scale feature in the tree.

Using the Dome Feature
The Dome feature in SolidWorks is generally applied to give some shape to flat faces or an area
of a flat face. A great example of where a dome fits well is the cupped bottom of a plastic bottle
or a slight arch on top of buttons for electronic devices. Domes can add or remove material.
Until SolidWorks 2010, another very similar feature existed, which was called Shape. You can
no longer make Shape features, but you may run into one from time to time in old parts. If you
find a Shape feature on an old part, it will continue to function unless any of its parent geometry
changes. Shape features do not update in SolidWorks 2010 or later. SolidWorks recommends you
re-create the geometry as another feature, possibly a Dome or Freeform feature. Included in the
sample parts for Chapter 8 is a part called Chapter 8 Domes.sldprt; this part is shown in
Figure 8.10. Opening this part will allow you to see the error that appears when you open a part
with a Shape feature. The part also demonstrates several ways in which Dome features
can be used.