The scope of this article is to highlight the use and benefits of Inheritance feature. The procedure below describes ONE of the methods using basic elements. However, the Inheritance method is the preferred one for such application.
Table 1 gives a comparison of Inheritance feature vis-à-vis Family Table and Copy Geometry.
|INHERITANCE FEATURE||FEATURE FAMILY||COPY GEOMETRY|
|Increased access to copied feature information; where in references to many elements are needed||Each instance of the family table includes characteristics of the whole family||Is more suited where only a few references are needed from an external model|
|Allows One-way merge of geometry and feature data from one part to another||Only geometry data is copied. Solid geometry will have to be created. Suited where the generic part itself is not needed or where further operations on the generic part will not be done to get a new part|
|Inheritance feature begins with all of its geometry and data IDENTICAL to the part from which it is derived, without changing the base model||References like surfaces, edges and axis are only referenced. A new Part is built using these references. This is more suited where the new part is very different from the generic part and the copied geometries are used for references only|
|Inheritance feature gives a BASE model associative to the generic model||This is similar in a Family Part|
|Inheritance features can contain varied dimensions from the model from which it has inherited||This is similar in a FAMILY PART. However, a Family Part will contain all the features of the Generic part listed in the Model tree. Family tables are useful where you need to create more than ONE variety, quickly, with the parameters entered in an excel sheet. When you change, a dimension carried from the GENERIC model, while in Instance mode, the parent part changes. This would not be desirable in some cases|
|Action items can be performed on an inheritance feature like modifying dimensions and suppressing features||This again is similar in a family part.|
|Allows a direct reference to the top-level skeleton with access to
all of its features
|Does not allow full access to all the feature information|
Procedure to design the casting
We would generally follow the steps given below to achieve the final product as shown in Fig.4
- Determine the machined surfaces and the machining allowance.
- In case we choose to give a constant machining allowance (could be a company standard), create a Parameter - for example "mc_allow" - and equate it to the machining allowance (Fig.1). This would allow global change for the machining allowance should it change at a later stage.
- Create Datum planes for the machined faces MAC_FACE_1, 2, 3 & 4. This can also be a copy geometry or a publish geometry from an assembly or other model.
- Create offset Datum planes from the machined surfaces offset by a distance equal to the machining allowance to get Cast_faces CF_1, 2, 3 & 4. At this stage, you may also equate the offset to “mc_allow”, created in Fig.1. Refer to Fig.2.
- To begin the design, sketch circles on planes for Protrusions. Refer to Fig.3.
- Now extrude the geometries to the Casting Planes CF_1, CF_2 etc.; to get a component as shown in Fig.4.
Procedure to design the machined version of the component
- Start a New Part say “Machined”.
- Insert > Shared data > Merge/Inheritance…
- Open the Casting part and place it to Default placement location.
- Add cut features using the "MAC_FACE_1, 2, 3 & 4" as reference planes.
Note! One needs AAX module for the commands.
You will get the component as given below, with the machined surfaces shown in RED. Ref: Fig.5. The rounds created in casting are in yellow after applying the machining cut.