Standard components are not only individual parts, but also assemblies of them. These assemblies usually contain free-form parts as well as parts with standardized shape. Regardless of the component type, its ideal definition should allow you to adjust the size and shape to the design requirements and its influence on the design context.
Consider the Fixture component (Fig. 18), which consists of two standardized parts (CapScrew ISO 4762 M10x75.1 and Sleeve Fw22/14×120.1) and one free-form part (Guide.1). Each change in the parameter values of this component initiates appropriate geometric changes of its elements (based on the NestingGuideDesignTable) and changes in component names for standardized parts (UnifyInstanceName reaction, which triggers the macro InstanceName equal to PartNumber).
![The fixture component with two standardized parts](https://about-engineering.com/wp-content/uploads/2022/01/designing-standard-components-18.jpeg)
Geometric definition of the Fixture component (Fig. 19) is based on the concept of the standard component, which I described in the previous part of this cycle. Both standard parts (here: Sleeve Fw22/10×80 and CapScrew ISO 4762 M8x55) have a defined impact on design context and thus, when they are inserted into the Fixture product in the Guide.1 component the system generates the appropriate holes:
- The DrillHole solid of the component Sleeve Fw22/10×80 defines the hole DrillHoleSleeve Fw22/10x80_1.1,
- The DrillHole solid of the CapScrew ISO 4762 M8x55 component defines the DrillHoleCapScrew ISO 4762 M8x55_1.1 hole,
- The TapHole solid of the CapScrew ISO 4762 M8x55 component has no effect on the Guide.1.
![The concept of standard components](https://about-engineering.com/wp-content/uploads/2022/01/designing-standard-components-19.jpeg)
Each one of these holes is the result of the Copy + PasteSpecial… As Result With Link command. If the fixing screw and positioning pin are inserted into the Fixture product structure using the Add User Component command (the command available in the Tooling Design 1 workbench of CATIA V5), the impact of these components on the shape of the Guide.1 part is defined automatically. Assembly Constraints relationships are also defined automatically, but (unfortunately!) the component positioning definition is incomplete. For example, the position of the CapScrew ISO 4762 M8x55.1 component relative to Guide.1 is only defined by one relationship (Offset.3 in Figure 20 A). If the screw insertion point (or points) was defined using a sketch (Sketch type object), the system would define two Offset type relationships.
![](https://about-engineering.com/wp-content/uploads/2022/01/designing-standard-components-20.jpeg)
This definition of the screw position is also not complete, which is easy to check with the Manipulation command (Assembly Design workbench) – despite the active With respect to constraints mode (Fig.20B) the system allows you to rotate the screw. For this reason, a complete and unambiguous definition of the Fixture component requires the intervention of the designer, who must define the missing relationships of the Assembly Constraints type (in this example – for the screw and dowel). If the influence of the Fixture component on the design context has to be defined not only for the screw and dowel, but also for the Guide component, its definition would have to be slightly modified. If in the Guide component we define a Pocket body (Fig. 21), then because its negative polarity, after inserting the Fixture component into any assembly, a pocket appropriate for the selected size will be made by the system automatically.
![](https://about-engineering.com/wp-content/uploads/2022/01/designing-standard-components-21.jpeg)