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Preparing the plastic part for Mold Tools

The Mold Tools process formally starts with identifying edges as parting lines. Before you get to that point, there are some things you have to do to the plastic part model, such as shelling the part, creating draft, and accounting for shrinkage.

For this example, you will use a part from the DVD (see Figure 21.3). This part uses a master model technique to create multiple parts from a single surface model, and then is inserted into a new part for the Mold Tools process, so three levels exist for the part. The one you are concerned with in this example is called Mold Tools medical device.sldprt, which contains a single feature, an inserted part called medical device frame.

FIGURE 21.3

The plastic part for the example in this chapter

Shelling the part and applying draft

Shelling and applying draft to a plastic part isn't something you can cover in a couple of paragraphs. Shell and draft features, including the evaluation techniques to determine the wall thickness, direction, and amount of the draft that was applied, are covered in detail in the SolidWorks 2011 Parts Bible (Wiley 2011).

Adding the plastic part to a blank part

The Mold Tools process works in multi-body mode rather than in assembly mode. This makes sense as long as you don't start by putting all of the Mold Tools features into the same file that contains all of the plastic part features. This would make a single part with many features that exist for different purposes.

The best practice to follow when preparing a part for Mold Tools is to insert the part into a new part using the Insert Part feature at the top of an empty new part. This does a couple of things. First, it gives you more control over the rebuild times for the Mold Tools from the rebuild times for the plastic part. In addition, if you are just working on the plastic part, you don't want to have to worry about the Mold Tools features. Second, it separates the features of the Mold Tools so you don't have to be working with the live plastic part data when all you need is the final geometry.

This step is just a recommended part of the process that has been added; it is not part of the process that SolidWorks has established for the tools, but you will probably find that it is useful.

Using the Scale feature

The Scale feature is used to make the plastic part slightly larger to compensate for plastic shrinkage during molding. Scale is driven by a multiplier value, so a part that is twice as big gets a scale factor of 2, and one that is half as big gets a scale factor of .5. Plastic materials have a shrink rate that is usually measured in thousandths of an inch per inch of part. Five thousands inch per inch is equal to a 0.005 scale factor. If the part is 4 inches long, the mold cavity to produce it must be 4.020 inches with that material.

Some materials have anisotropic shrink rates, meaning they shrink different amounts in different directions, with the primary direction being considered the direction of the molten plastic through the mold cavity. SolidWorks has a means to compensate for this, although it may not always be practical. Usually the shrink directions are identified as “in the direction of flow” and “across the direction of flow,” and the direction of flow of molten plastic inside a mold cavity is not always a straight line. Any anisotropic shrink applied to a part in SolidWorks is an approximation at best. If you deselect the Uniform scaling option in the Scale feature, SolidWorks enables you to set different scale factors for X, Y, and Z directions. The Scale PropertyManager is shown in Figure 21.4, in both its Uniform Scaling and non-Uniform Scaling configurations.

FIGURE 21.4

The Scale PropertyManager

Where you should put the Scale feature is debatable. Some people argue that it should be placed in the plastic part file, so that it is ready to create the mold geometry. Others believe it should be placed in the part file that the mold tools are created in, because you might design a mold for polypropylene differently