4.6.3 Associations

In the previous chapters you have learned how to create a solid model with features like sketches, production operations, etc. You have also learned how to use Parametric Design in this context. Among other things, this opens up various possibilities for realizing more specific design and functional elements of components. The following section describes an example of a sketch- and feature-based approach, taking into account the relationships between different elements and their interrelationships (associations). As an example, a very simple parametric shaft with two keyways shall be used. One requirement is that the feather keys always lie in the middle of the two shaft ends (refer figure "Shaft").

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First create a new part with the name features_and_sketches according to the naming convention.

Then create the necessary parameters for the shaft. For example, you can define the following parameters:

In the following, you will create the keyway once using the Slot feature and then using the sketch-based approach. Therefore, first create an auxiliary plane on the shaft end. The Tangent option in the Datum Plane dialog is useful here. For the Subtype option, choose Through Point.In addition to the cylindrical surface, select an auxiliary point to define the position of the auxiliary plane on the cylindrical surface. The option Quadrant Point under Specify Point, for example, is suitable for this (refer figure "Varying the auxiliary plane").

For a sketch-based approach, an analogous procedure is the first one in which you use a tangential auxiliary layer to place the sketch. Then you create the shape of the groove using a sketch (refer figure "Sketch"). Always make sure that the sketch is fully constrained. Then apply the parameters to the dimensions of the sketch. After completing the sketch, use the Extrude feature and subtract the extruded body from the fundamental shaft to obtain a symmetric shaft (refer figure "Shaft").

How good a parametric construction is can usually only be seen when the parameters change. First vary the parameters by the length, width and depth of the keyway to determine the effect on your construction. If the width exceeds the length of the feather key this leads to an error of the Slot feature, because this is not allowed by the definition of the feature. However, your sketch-based design should allow this, even if it doesn't do any greater good here. Then make sure that the feather keys are always centered on the shaft ends by varying the dimensions of the shaft. Afterwards you should not only try to change the parameters directly, but also vary the position and orientation of the keyway or auxiliary plane with which it was created by moving the position of the tangential surface e.g. to the opposite side (refer figure "Varying the auxiliary plane").

You will notice that errors occur in the case of the sketch. The reason for this is the orientation of the sketch or its coordinate system. The normal vector of the cylindrical surface forms the basis for the orientation of the internal coordinate system of the sketch. The origin of this coordinate system and the second direction vector have not yet been explicitly defined, analogous to Auto Constraints in sketches. To correct this error, first create a parametric auxiliary point using Point , as you will reference it in two places below (refer figure "Auxiliary point"). To use the auxiliary point for creating the auxiliary plane, move it in thePart Navigator before the auxiliary plane. Change the auxiliary level to use the created auxiliary point (refer figure "Varying the auxiliary plane"). Then, edit the sketch and run the Reattach command. Then select the created auxiliary point for the origin (refer figure "Defining the origin"). Define the second direction vector of the coordinate system, look at the coordinate system of the sketch again (refer figure "Defining the origin"). This orientation should be retained, otherwise the following errors will occur. Now set the reference for the orientation of the sketch to Vertical (y-axis). The orientation of the coordinate system will change first. As reference for the y-axis you now choose the top surface of the shaft end, as this represents the rotation axis (refer figure "Defining orientation"). The orientation should now correspond to the original again. Confirm the result with OK and leave the Sketch environment. Your part should not have changed. Now change the position of the created auxiliary point. Now no errors should occur when changing the position of the help point on the edge (refer figure "Changed Shaft")

A big advantage of features is obviously their robustness, but their shape is always determined by their definition. For example, NX has only a limited number of predefined features by default. By default, these are mainly the features presented in this tutorial. More specific design elements such as disk springs or hyperbolide gears cannot be constructed sensibly with the standard features. This shows the advantage of sketches. This allows you to create virtually any body. In particular, however, with parameteric constructing of construction units, you must consider however clearly more associations between the different elements in their construction.