Create derived part or assembly

You can create a derived part using a part, assembly, sheet metal part, or weldment. The source is called the base component in the new file. You can include or exclude bodies or components, work features, sketches, constraints, iMates, and parameters in a derived part. When deriving an assembly, you can also specify representations (Design View, Positional, and Level of Detail).

A derived part or assembly may be a scaled, mirrored or simplified version of the original.

Derive a part

Select features, bodies, surfaces, visible 2D and 3D sketches, work features, parameters, and iMates to include or exclude from the derived part. Sketches that are not shared or consumed by features are included in the base component. If the source part is a multi-body part you can also specify whether the derived component becomes a single body solid, a multi-body solid, or a surface in your new file.

To begin, create a part file. If you want to create a multi-body part file, create one or more features or bodies. If you want to create a part with no pre-existing features or bodies, choose Finish Sketch when you start the new part to close the default sketch.

1. On the ribbon, click Manage tab Insert panel Derive .
2. In the Open dialog box, browse to the part file (.ipt) to use as the base component, and then click Open.
3. Select the Derive style.

   Creates a single solid body derived part with no seams between planar faces.

   Creates a single solid body derived part with seams between planar faces.

   Creates a derived part with one or more solid bodies if the source part contains multiple bodies. This is the default option.

   Creates a derived part with a single surface body.

4. In the Derived Part dialog box, model elements are displayed in a hierarchy. Accept the default or use the Status buttons at the top to change the status of all selected objects quickly. You also can click a status icon next to an individual object and toggle the status options.

   If the source part contains only one body, it is displayed in the graphics screen. If the source part is a multi-body part with only one visible body, it is displayed in the graphics screen. If the source part is a multi-body part with more than one body visible, no bodies are displayed in the graphics screen. To specify the body or bodies to include, expand the Solid Bodies folder and use the Status button to include or exclude bodies. If you want to include all bodies, you can select the Solid Bodies folder and then click the include status button.

   Note: Only bodies that are visible in the source part file are selectable.

   Selects element for inclusion in the derived part.

   Excludes element in the derived part. Items marked with this symbol are ignored in updates to the derived part.

   Note: If you select a nonexported object for inclusion in the derived part, a confirmation message appears when you close the Derived Part dialog box notifying you that the base file marks the object for export.
5. If required, click Select from Base to allow graphical selection of components from the base component window. After you select the components, click Accept Selection .
6. If required, turn off the Show All Objects check box to display only exported elements in the list.
7. Specify scale factor and mirror plane:
   • Accept the default scale factor of 1.0 or enter any positive number.
   • If required, select the check box to mirror the derived part feature from the base part. Click the down arrow to select an origin work plane as the mirror plane.
8. Click OK.
   Note: If you select a geometric group, such as surfaces, for inclusion in the derived part, any visible surface later added to the base part is derived when you update. After placing the derived part in an assembly, click Update to regenerate only the local part and click Global Update to update the entire assembly.

Derive an assembly

A derived assembly component originates from an assembly file and may contain parts, subassemblies, and derived parts. You select geometry to add, subtract, or exclude from the resulting derived component. You may also include or exclude sketches, work geometry, and parameters.

Tip: So you can see which components are included, excluded, or subtracted, geometry changes color in the graphics window to match the symbol status on the Bodies tab of the dialog box.

To begin, create a part file, and then click Return to close the default sketch.

	On the ribbon, click Manage tab Insert panel Derive . In the Open dialog box, browse to the assembly file (.iam) to use as the base component. Click Options to specify the representations to use in the derived component and then click OK to close the File Open Options dialog box. Click Open to close the Open dialog box. Note: If you want to use a Level of Detail representation, specify it in this dialog box. It cannot be changed later in the derived component. Select the Derive style. Creates a single solid body derived part with no seams between planar faces. This is the default option. Creates a single solid body derived part with seams between planar faces. Creates a derived part with one or more solid bodies if the source part contains multiple bodies. Creates a derived part as a single surface composite which retains the appearance of the original components. Creates the smallest file on disk.
	In the Derived Assembly dialog box, assembly components display in a hierarchy. On the Bodies tab, accept the default or use the Status buttons at the top to change the status of all selected components quickly. Tip: To select all parts in the subassembly quickly, right-click a parent node in the tree and choose Select All Parts from the context menu. You also can click a status icon next to an individual component and cycle through the status options. Note: If the Associative check box is selected in the Representations tab, you cannot exclude components that are visible in the specified Design View. Selects component for inclusion in the derived part. Excludes component from the derived part. Items marked with this symbol are ignored in updates to the derived part. Subtracts component from the derived part. If the subtracted component intersects with the part, the result is a cavity. Represents the selected component in the derived part as a bounding box and creates a body from the bounding box shape. The reduced detail decreases memory consumption. Intersects the selected component with the derived part. At least one component must have an Include status. If the component does not intersect the derived part, the result is no solid. If required, click Select from Base to allow graphical selection of components from the base component window. After you select the components, click Accept Selection . If required, select the check box to keep seams between planar faces.
	Click the Other tab to select sketches, work geometry, and parameters. You cannot subtract elements from the derived body on the Other tab. If desired, turn off the Show All Objects check box to display only exported elements in the list. Click the Representations tab to select a Design View, Positional, and Level of Detail representation. If you selected them on the File Open Options dialog boxes, your selections are listed, but you can select alternate representations from the lists. Design View representations are associative by default, but you can turn off the associative check box so that the modifications to a design view do not affect the derived assembly. Click the Options tab to select Simplification if required. You can remove geometry by visibility and size to simplify the part. For example, a setting of zero visibility means that components that are completely hidden in any view will be removed. Select the Hole patching options if required. Specify scale factor and mirror plane: Accept the default scale factor of 1.0 or enter any positive number. If desired, select the check box to mirror the derived part feature from the base part. Click the down arrow to select an origin work plane as the mirror plane. If appropriate, select the Reduced Memory Mode check box to significantly reduce the browser data stored in the part. Overall memory reduction is dependent on the complexity of the assembly. A surface composite does not cache any of the source bodies. Select Create independent bodies on failed Boolean to create a multi-body part when a Boolean operation fails on one of the single solid body style options. Select Remove All Internal Voids to fill all internal void shells in the derived solid body part. Verify that you have selected needed bodies, sketches, work geometry, parameters, and representations, and then click OK. Note: If a subassembly is selected for addition or subtraction, any component later added to the subassembly is automatically included when you update. After placing the derived part in an assembly, click Update to regenerate only the local part and click Global Update to update the entire assembly.