SolidWorks 2011 Parts Bible - Matt Lombard [56]
FIGURE 3.35
Creating a new plane from a set of selections and constraints
The good news about this method is that there are far more options for creating planes than in the previous method, but the bad news is that the options are not all spelled out anywhere. You have to make a selection before it shows you the available constraints. The older interface presented the available options right up front, but there were fewer to choose from. Hopefully this interface matures in the future. Meanwhile, you may need to experiment to see what works best for the type of modeling you do.
Note
For longtime users, when you start using the new Plane functionality, it may be best to try to ignore the new interface and simply make the same types of selections that you made in the past. The new Plane functionality will work perfectly that way. If you are a new user, just think of how you would like to specify the new plane, given the available geometry, and give it a try. The available options are not documented, so working with this interface requires some blind trust on the part of the user. The tool is quite powerful, but you will need to spend time experimenting with it. Even then, you will be unsure whether you are missing important options.
Working with axes
You can use axes to create pivot points in a part where you do not have any hole-type geometry for mating with other parts, or as a direction of pull for plastic parts or molds. Axes are frequently used to establish direction. Figure 3.36 shows that the first three features in a plastic part are axes established from the standard planes.
FIGURE 3.36
Using axes to establish direction
Consider using axes set up in this way as standard features in your template files. They can be effective in assemblies for moving parts in orthogonal directions and in parts for pattern or draft directions.
Note
The interface for the Axis feature has not been changed to match the Plane interface. Notice that the methods for creating an axis are spelled out clearly in the interface. I expect to eventually see a change to Axis to make it match the Plane interface.
Using Coordinate Systems
Coordinate Systems in SolidWorks are primarily used for import and export, but can also be used for mating, mass properties, and other purposes. Coordinate Systems are usually located by a point to determine location or a set of edges to determine direction. Figure 3.37 shows the PropertyManager for assigning a coordinate system, along with the Export Options dialog box, which you can access from the Save As dialog box when the Files of Type drop-down is set to an export format.
FIGURE 3.37
Use Coordinate Systems to export parts and assemblies with a new origin location.
To use the coordinate system when saving as a translated file type such as IGES or Parasolid, click the Options button, as shown in Figure 3.37; at the bottom of the Export Options dialog box, a selection box for Output coordinate system appears.
To use the coordinate system with mass properties, choose Tools⇒Mass Properties from the menu, and then select the Output coordinate system, as shown in Figure 3.38.
FIGURE 3.38
Assigning the coordinate system with a well-hidden setting
Using points as reference geometry
The Point reference geometry feature is infrequently used; however, in some situations there is nothing else that does the job quite as well. This is not the same as a sketch point and does not require a sketch to be open; it is just a reference point that you can place in space. Figure 3.39 shows the PropertyManager for the Point reference geometry feature.
FIGURE 3.39
The Point reference geometry feature has several modes of point creation you won't find elsewhere.
My favorite Point placement method is the Along Curve Distance option (the bottom one in Figure 3.39). It enables you to create several regularly spaced points along a curve.
Tutorial: Learning to Use