To Create a 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. 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.

What's New: 2020.1, 2021.1, 2022

Create a Derived 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.

  1. 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 single solid part with no pre-existing features or bodies, choose Finish Sketch when you start the new part to close the default sketch.
  2. On the ribbon, click Manage tab Insert panel Derive .
  3. In the Open dialog box, browse to the part file (IPT) to use as the base part or component, and click Open.
  4. 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.

    If the base part contains a single body, creates a single body part. If the base part contains multiple visible solid bodies, select the required bodies to create a multi-body part. This is the default option.

    Creates a derived part with a single surface body.

  5. 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.

    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.

  6. If the base 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.
    Note: Only bodies that are visible in the base part file are selectable.
  7. If necessary, click Select from Base to allow graphical selection of components from the base component window. After you select the components, click Accept Selection .
  8. If necessary, turn off the Show All Objects check box to display only exported elements in the list.
  9. Specify scale factor and mirror plane:
    • Accept the default scale factor of 1.0 or enter any positive number.
    • If necessary, select the check box to mirror the derived part feature from the base part.
      Note: Sketch block instances of selected block definitions are mirrored. However, the block definitions are not mirrored.
  10. If necessary, check the Use color override from source component check box to link the color from the base component into the target part. If unchecked, the appearance is set to default appearance of the target part.
    Note: A setting can be configured to default the Use color override from source component check box to remain checked or unchecked throughout your session. This check box can be accessed through the Application Options dialog box in the Part tab.
  11. 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.

Create a Derived Part from an Assembly

You may also include or exclude sketches, work geometry, and parameters.

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

  1. To begin, create a part file. If a sketch is active when you create the part, click Return to close the sketch.
  2. On the ribbon, click Manage tab Insert panel Derive .
  3. In the Open dialog box, browse to the assembly file (.iam) to use as the base component.
  4. Click Options to specify the model state and 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.
  5. 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 multi-body part that retains selected components as individual solid bodies. For example, an assembly with five parts creates a part with five solid bodies.

    Creates a derived part as a single surface composite which retains the appearance of the original components. Creates the smallest file on disk.

  6. In the Derived Assembly dialog box, assembly components appear 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.
    Note: If Associative check 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. (Suppressed components are excluded; this cannot be changed. Dependent components of a suppressed component are not listed.)

    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. The bounding box updates to reflect changes in the derived component or in the base component.

    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.

  7. If necessary, click Select from Base to graphically select components from the base component window. After you select the components, click Accept Selection .
  8. If necessary, select the check box to keep seams between planar faces.
  9. Click the Other tab to select sketches, work geometry, and parameters.

    Only iMates for top-level assemblies may be derived. If one of the iMate participants is a bounding box, it is a new body and the face is no longer available. (The iMate may be used, but not edited.)

    If desired, turn off the Show All Objects check box to display only exported elements in the list.

  10. Click the Representations tab to select a Model State, Design View, or Positional representation. If you selected them on the File Open Options dialogs, you can change them here.

    The Design View representation affects the status of components in the Body tab. For example, an occurrence that is invisible is set to Exclude. Disabled components remain included, however.

  11. Click the Options tab to select Simplification if necessary. 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.
  12. Select the Hole patching options if necessary.
  13. 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.
  14. Check the Use color override from source component check to link the color from the base component into the target part. If unchecked, the appearance is set to default appearance of the target part.
    Note: A global setting can be set to default the Use color override from source component check box to remain checked or unchecked throughout your session. This check box can be accessed through the Application Options dialog box.
  15. If appropriate, select the Reduced Memory Mode to significantly reduce the browser data stored in the part. Overall memory reduction depends on the complexity of the assembly. A surface composite does not cache any of the source bodies.
    Note: A surface composite does not cache any of the source bodies. Also, Reduced Memory Mode is unavailable if you chose the derive style Maintain Each Solid as a Solid Body.
  16. 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.
  17. Select Remove All Internal Voids to fill all internal void shells in the derived solid body part.
  18. 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.

Create a Derived Substitute Part from an Assembly

You can create an assembly substitute part from within an assembly to increase performance and capacity.

  1. On the browser, right-click either the Model States folder or a model state entry below and select New Substitute Derive Assembly.
  2. In the New Derived Substitute Part dialog box, specify:
    • New Component Name
    • Template
    • New File Location

    3. Click OK to finish.

  3. Start at step 5 in the preceding section and follow the remaining steps to complete the workflow.
Note: The Associative link setting in the Derived Part and Derived Assembly dialog boxes persists across sessions of Inventor. For example, if you select the checkbox, the checkbox remains selected the next time you access the dialog box in the same and future sessions of Inventor.
Parent topic: About Derived Parts and Assemblies