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The Scale Factor works like a multiplier, so if you want to double all the dimensions, 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, so to double the linear dimensions of a part would require a scale factor of 100%. The Cavity feature is only available in the context of an assembly, and has fallen out of favor with most mold designers.

Scale is also configurable, starting with SolidWorks 2011, meaning that different configurations can use different scale factors. Configurations are covered in Chapter 11.

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 dimensions, 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 approximately a box of between 500 and 700 meters centered around the origin. There appears to be some difference between sketching limits and 3D solid limits.

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.

Until SolidWorks 2010, another very similar feature existed, which was called Shape. You can no longer make Shape features, but you may find 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 will not update in SolidWorks 2010 or later. SolidWorks recommends you re-create the geometry as another feature, possibly a Dome or Freeform feature.

Best Practice

Dome features are best used when you are looking for a generic bulge or indentation and are not too concerned about controlling the specific shape. Occasionally, a dome may be exactly what you need, but when you need more precise, predictable control over the shape, then you should use the Fill, Boundary, or Loft feature.

The Dome feature has several attributes that will either help it qualify for a given task or disqualify it. These attributes can help you decide if it will be useful in situations you encounter:

• The Dome feature can create multiple domes on multiple selected faces in a single feature, although it creates only a single dome for each face.

• Using the Elliptical Dome setting, Dome can create a feature that is tangent to the vertical.

• Dome can use a constraint sketch to limit its shape.

• Dome works on non-planar faces.

• Dome cannot establish a tangent relationship to faces bordering the selected face.

• Dome cannot span multiple faces.

• Dome displays a temporary untrimmed four-sided patch that extends beyond the selected face when you use it on a non-four-sided face.

• Dome