To Copy Objects Between Part, Assembly, and Construction Environments

You can copy or move geometry within a part file to composites, base surfaces, a repair body or a group in the construction environment.

What's New: 2021

Copy Objects Associatively Between Parts in Assembly (not available in Inventor LT)

When editing a part file within the assembly, you can copy geometry from one part to another, associatively, as a surface or composite feature. These features update automatically when updates are made to the original source data.

1. In an assembly file, double-click the part to edit. The part environment and commands become available.
2. On the ribbon, click 3D Model tab Modify panel Copy Object .
3. Alternately, if you are in the Construction environment, click Construction tabManage panel Copy Object.
4. Select the Input Geometry:
   • Faces selection, the default, is active.
   • Click Body selection to select one or more body, solids, quilts, or surfaces.
5. Specify the Output options:
   • Method
     • New Object. Creates a new object.
     • Join. Select an existing object. The new object is part of the selected object.
   • Object
     • Composite is selected by default. The Composite option creates one composite feature in the browser for the entire selection set.
     • Surface creates a Base Surface feature for every body or every set of contiguous faces of a single body selected.
6. In the graphics window, select the geometry to be copied as a new feature.

   To maintain an adaptive relationship with the source part, ensure the Associative check box is selected. Leave it unselected if association is not needed.

   Note: You can only select the type of geometry specified as the selection option (Face or Body).
7. Click Apply to complete the specified action without closing the dialog box. Click OK to complete the specified action and close the dialog box.
8. To remove the associativity, do any of the following:
   • To remove the associativity temporarily between the source and the feature created with Copy Object, right-click on the Surface or Composite entry in the browser, and cancel the Adaptive selection.
   • To reset the relationship back to Associative, select Adaptive in the context menu again. Selecting Adaptive in the context menu acts as an On/Off toggle.
   • To permanently remove the associativity between the source and the feature created with Copy Object, right-click the Surface or Composite reference entry in the browser, and then select Break Link.
   Note: Cancel the selection of the Associative option to create a single non-associative copy of geometry from another part in an assembly.

Create Repair Body

1. In a part file that contains features, click 3D Model tab Modify panel Copy Object .
2. Select the Input Geometry:
   • Faces selection, the default, is active.
   • Click Body selection to select one or more body, solids, quilts, or surfaces.
3. Specify the Output options:
   • Method
     • New Object. Creates a new object.
     • Join Existing. The new object will be part of the selected object.
   • Object
     • Composite is selected by default. The Composite option creates one composite feature in the browser for the entire selection set.
     • Surface creates a Base Surface feature for every body or every set of contiguous faces of a single body selected.
4. Click OK to finish.
5. Click 3D Model tab Surface panel Repair Bodies .
6. Select the composite or surface in the browser to create a new repair body.

Copy Face or Body to Existing Repair Body

You can use copy object to copy a face or body to an existing repair body.

1. In a part file that contains features and a repair body, click 3D Model tab Modify panel Copy Object .
2. Select the Input Geometry:
   • Faces selection, the default, is active.
   • Click Body selection to select one or more body, solids, quilts, or surfaces.
3. In the Output section, click Join Existing and then select the repair body.
4. Click OK to finish.

Copy or Move Objects from Construction Environment

You can create a copy or move geometry from the construction environment as a surface or composite within a part file.

1. In the construction environment, click Construction tab Manage panel Copy Object in a part (.ipt) file.
2. Select the Input Geometry:
   • Faces selection, the default, is active.
   • Click Body selection to select one or more body, solids, quilts, or surfaces.
3. Specify the Output options:
   • Method
     • New Object. Creates a new object.
     • Join Existing. The new object will be part of the selected object.
   • Object
     • Composite is selected by default. The Composite option creates one composite feature in the browser for the entire selection set.
     • Surface creates a Base Surface feature for every body or every set of contiguous faces of a single body selected.
4. To move (instead of copy) the selection, ensure that Delete Original is selected. To copy the selection, cancel the selection of Delete Original.
5. In the graphics window, select the geometry to be copied or moved as a new feature. Geometry can be selected from the construction environment or from the part environment.
6. Click OK.

Note: The Delete Original command does not delete Parametric geometry from the original location, only base features.

Copy or Move Objects from Part Modeling Environment

You can copy or move geometry between the construction environment and the part modeling environment as a group feature.

1. Click Construction tab Manage panel Copy Object in a part (.ipt) file.
2. Select the Input Geometry:
   • Faces selection, the default, is active.
   • Click Body selection to select one or more body, solids, quilts, or surfaces.
3. In the Output section, select the Group option.
4. In the graphics window, select the geometry to be copied, or move to the construction environment.
5. To move the selection to the construction folder, ensure that Delete Original is selected. To copy the selection, cancel the Delete Original selection.
6. Click OK

The newly created group displays in the browser in the construction folder.

Note: The Delete Original command does not delete Parametric geometry from the part modeling environment.