Use Copy Object to copy or move geometry within a part file to composites, base surfaces, or a group in the construction environment. For example, you can create a copy or move geometry between the construction environment and the part modeling environment.

Copy Object and solid geometry

You can copy a solid to the part environment by using the Derive command..

If the original geometry changes size or position, the copied geometry does not update.

Copy Object and the construction environment

Use Copy Object to copy and/or move data between the construction and part modeling environment.

For example, when importing data from a file that contains multiple bodies, such as surfaces and solids, you may have to move surfaces to the construction environment to be stitched together to form a single part. You can use Copy Object to copy or move faces (or solids) to the construction environment, and then stitch the faces together to form a part. You can then copy or move the data back to part modeling using the Copy Object command.

One possible workflow:

Open a translated file, and click Construction tabManage panel Copy Object.
Select the faces you want to copy or move, and select the Group option. Copy the selected faces to the construction environment.
Now that these faces are in the construction environment, use the Stitch command to stitch the faces together.
You can use Copy Object to copy or move the data back to part modeling.

Procedures

Copy object

Click here for information on: Add, Remove, and Redefine.

Use Copy Object to copy or move geometry within a part file to composites, base surfaces, a repair body, or a group in the construction environment. For example, you can create a copy or move geometry between the construction environment and the part modeling environment.

Use Copy Object to create a repair body

You can use copy object to create a base body and then create a new repair body.

In a part file that contains features, click 3D Model tabModify panel Copy Object.
Select the required faces or body.
The Composite output option is selected by default. The Composite option creates one composite feature in the browser for the entire selection set.
The Surface option creates a Base Surface feature for every body or every set of contiguous faces of a single body selected.
Click OK to finish.
Click 3D Model tabSurface panel Repair Bodies .
Select the composite or surface in the browser to create a new repair body.

Use Copy Object to copy a face or body to an existing repair body

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

In a part file that contains features and a repair body, click 3D Model tabModify panel Copy Object.
Select the required faces or body.
In the output pane, click Select Existing and then select the repair body.
Click OK to finish.

Copy or move objects from the construction environment to the part modeling environment as a surface or as a composite

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

In the construction environment, click Construction tabManage panel Copy Object in a part (.ipt) file.
Select the type of geometry:
- Choose Face to select one or more faces on the part.
- Choose Body to select one or more body, solids, quilts,or surfaces.
The Composite output option is selected by default. The Composite option creates one composite feature in the browser for the entire selection set.
The Surface option creates a Base Surface feature for every body or set of contiguous faces selected.
To move (instead of copy) the selection, ensure that Delete Original is selected. To copy the selection, cancel the selection of Delete Original.
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.
Click OK.
The newly created feature displays in the browser as a Composite or Base Surfaces feature.

Composite feature displays in browser

Surface features displays in browser

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

Copy or move objects from the part modeling environment to the construction environment as a group feature

You can copy or move geometry between the construction environment and the part modeling environment.

Click Construction tabManage panel Copy Object in a part (.ipt) file.
Select the type of geometry:
- Choose Face to select one or more faces on the part.
- Choose Body to select one or more body, solids, quilts,or surfaces.
Select the Group output option.
In the graphics window, select the geometry to be copied, or move to the construction environment.
To move the selection to the construction folder, ensure that Delete Original is selected. To copy the selection, cancel the Delete Original selection.
Click OK

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

NoteThe Delete Original command does not delete Parametric geometry from the part modeling environment.

Additional workflow notes:

You can create a new composite feature with no geometry as a placeholder for geometry to be copied at a later time. Open the Copy Object dialog box, and click OK.
You can select the existing group or composite feature to which you are adding geometry. In the Copy Object dialog box select the Select Existing option, and then select an existing group or composite feature from the browser and click OK.
You can copy a solid to the part environment if the destination file does not already contain a solid.
For example, you can copy or move a solid from construction environment to the part modeling environment.

Promote wires to part environment

You can promote construction environment wire data to 3D sketches using either of the following two methods:

Method 1

Expand the Construction folder to display a Wires subgroup node in the browser.
Right-click the Wires subgroup node, and select Promote Wires.

The promoted wires are placed in a new 3D sketch in part modeling.

Method 2

Change the selection mode to Wires on the Quick Access toolbar.
In the graphics window, select the wires to promote to the part modeling environment.
Right-click, and select Promote Wires.

The selected wires are promoted to a 3D sketch in part modeling.

NotePromoted wires lose their original color when promoted to part modeling.

Generate wires from composite in 2D and 3D sketches

You can generate wire data using a composite feature, from the intersection of planes, in both the 2D and 3D sketches.

Generate wire from composite in 2D sketch

Import surface data to a composite feature.
Place a 2D sketch which intersects the composite.
In the sketch, click Sketch tabDraw panel Project Cut Edges from the ribbon.
Select the composite feature.

Curves are generated at the intersection of the sketch plane and any surface that crossed the plane. The curves update when the sketch is moved.

Generate wire from composite in 3D sketch

Import surface data to a composite feature.
Generate a surface which intersects the composite feature.
Start a new 3D sketch.
In the 3D sketch, click 3D Sketch tabDraw panel Intersection Curve from the ribbon.
Select the composite and the surface.
Click OK.

3D curves are generated in the 3D sketch at the intersection point. Curves update when intersection bodies are updated.

NoteEndpoints of the wires are not constrained. Offset behavior may be inconsistent.

References

Copy Object

Access:

Ribbon: 3D Model tab

Modify panel

Copy Object

Ribbon: Construction tab

Manage panel

Copy Object

Available in a part (.ipt) file or in an assembly (.iam) file when editing a part within the assembly context.

Click here for information on: Add, Remove, and Redefine

Use Copy Object to copy or move geometry within a part file to composites, base surfaces, or a group in the construction environment.For example, you can create a copy or move geometry between the construction environment and the part modeling environment..:

Select	Select: Allows selection of one or more faces or bodies. NoteSwitching between selection types (Face and Body) clears the selections set. Face: Allows selection of individual faces of a quilt or solid body. Body: Allows selection of an entire quilt or solid body.
Output	Create New: Select one of the following options to copy or move composites, surfaces, or solids. The selection (Face or Body) determines the available Output options. Group: Copies/moves the selection set to a new Group in the construction environment. Surface: Copies/moves the selection set to one or more base surface features in the Part Modeling environment. Creates one feature for each set of contiguous faces selected. Composite: Copies/moves the selection set to a single composite feature in the Part Modeling environment. Solid: Copies/moves the selection set to a single solid body in the Part Modeling environment. Multiple Solids: Copies/moves the selection set to multiple solid bodies in the Part Modeling environment. Select Existing: Allows the selection of a target repair body, composite feature or group. Delete Original: Deletes the geometry in the original location (Moves the selected geometry to the specified location). Not available when selecting geometry from a different part. NoteThe Delete Original command does not delete Parametric geometry.
Apply	Completes the specified action without closing the dialog.
OK	Completes the specified action and closes the dialog box when selections are complete.

Promote wires

Promotes construction environment wire data and moves it to 3D sketches.

Access:

In the construction environment under the Construction folder, select a Wire subgroup node from the browser, then right-click and select Promote Wires.

Promote Wires

Promotes and moves construction environment wire data to 3D sketches.

Inventor LT

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Copy and move geometry

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