Efficiency drives successful projects, and in life, you should never spend time reinventing the wheel—or remodeling the same part! Mastering the various copy tools in Autodesk Inventor is one of the fastest ways to reclaim your design time. So here are the essential techniques for copying at every level of your model, ensuring your design process remains efficient, accurate, and professional.
[This work is my own, but I did reference the Inventor help; it’s a great resource! And I used Quillbot to help with the grammar and Audiate for the video voiceovers.]
Mastering Sketch Object Duplication in Autodesk Inventor
Within the sketch environment, we shall start with the go-to classic… copy & paste. You can select objects, Ctrl + C, and Ctrl + V to create a copy. Inventor pastes the object to the cursor location. You will find copy and paste on the right-click menu as well.
You can paste the copied object into other sketches in the model or into other parts. Here I’ve already copied the slot geometry. Let’s create a new sketch and paste it. I will then need to move, rotate, and/or dimension it to place it in the desired location.
Inventor maintains the dimensions and constraints of the objects contained in the operation. It will not, however, bring with it dimensions or constraints to objects that are not being copied. Which makes sense. It won’t create dangling dimensions.
Fun fact, you can actually copy AutoCAD objects and paste them into an Inventor sketch. The conversion happens in real time. It’ll even bring dimensions across and convert them to Inventor parametric dimensions. [This might work from other 2D CAD applications too; I’ve just never tried it.]
Bonus Tip: When pasting in AutoCAD geometry, it comes unconstrained. You can, however, use Auto Dimension with Dimensions turned off to apply easy constraints like horizontal, vertical, perpendicular, and parallel.
For more precision on placing the copied objects, consider using Copy (or Move). To copy geometry in a sketch, select the objects and then pick a base point. This base point becomes the point you are moving from. You can then snap to other objects or along the closest vertical and horizontal axes.
Or by using the Precise Input toolbar, you can specify exact movements.
What else?
- Turn on Optimize for Single Selection to automatically switch to Base Point mode immediately after you make a single selection.
- As already discussed, Precise Input turns on the Precise Input toolbar so that you can specify locations by entering specific X and Y coordinates.
- Use the Clipboard to copy the selected geometry to the clipboard. This allows you to paste the selected geometry into a different sketch. This is the same as Ctrl + C and Ctrl + V
Move & Rotate also have a Copy option. This means you can create new geometry instead of changing the existing geometry.
Opposed to specific sketch objects, you can also copy entire sketches. This works even if the sketch is consumed in a feature, such as an extrusion. The easiest method is copying the sketch from the browser. This puts it into the Windows clipboard, so you can paste it in the active model or in a different model.
Again, Inventor will bring in the dimensions and constraints of the objects contained within the selection. It will not bring the dimensions and constraints across to other objects. For example, dimensions from the sketch geometry to the edge of the part are not included with the copy. Why? There’s no way that Inventor could re-associate the dimension correctly without guessing. So, in most cases, you will need to add dimensions or constraints to position the sketch appropriately.
Starting with Inventor 2024.1, when pasting a copied sketch, you have two options. Use Paste with Formulas to include user-defined parameters in the paste action. Parameters associated with the source sketch are copied and pasted without being duplicated. Note, Paste with Formulas is only supported within the same document, not across documents.
Bonus Tip: Pasted sketch coming in upside down and backward? You can flip the normal direction on non-origin work planes.
How to Efficiently Copy Part Features in Inventor
Like sketch entities, you can also copy part features and paste them to create copies.
Pasting a feature initiates Paste Features. This process is like inserting an iFeature, but without configuring the size. Newly copied features are fully independent.
By default, dependent features are not copied, only the selected features. For example, the fillet on the edge of a hole is not included by default. However, by changing Paste Features to Dependent the dependent features (like the fillet) are included.
Inventor uses unresolved plane references to position the features. For each selected feature you need to select the face or plane for insertion. Yes, this might mean picking the same face multiple times, but it also provides the ability to paste features to different faces.
Use the compass icon to drag the feature to a new position and the circular arrow arc to rotate it. You can also specify the angle in the dialog. Use the toggle to flip the direction.
With the parameters, you have the option of copying them independently or dependently. When using the dependent option, it uses the existing parameter. When using independent, Inventor creates new parameters.
The Art of Copying Inventor Components
Save As (and Replace Reference)
Save As is one of the easiest, if not the easiest, methods for creating duplicates. With the file open, pick Save As from the File menu, pick the location, and set the name, and you now have an independent copy you can change.
With an assembly, this method will not create copies of the subcomponents, but it doesn’t mean that you can’t add and remove components and adjust positions.
You can also do the same from the file explorer. Copy and paste the file to create the duplicate.
Now, what about the drawing?
For example, if I have part A and its associated drawing A, I copy both to create part B and drawing B. However, drawing B still references part A.
However, from drawing B, I can use the Replace Reference feature to update the drawing so that it points to part B instead. If you have already made changes to part B before opening the drawing, you might find that some dimensions or annotations are affected. But a bit of cleanup is still better than redoing the entire drawing!
The Replace Reference feature is also available in presentations (IPN) starting with Inventor 2027, allowing you to fix the associativity from the assembly to the presentation and then to the drawing.
Save and Replace
From the assembly you can use the assembly bonus tool, Save and Replace, to make an in-place copy of the component. This automates the process of saving a copy and replacing the instance within the assembly. Because it’s a copy of the component, Inventor maintains all relationships.
This works on both sub-assemblies and parts. After picking the component, you set the save location and set the name for the new file.
Save and Replace All is the same, except it replaces all instances of the component in the assembly with the newly created copy.
Streamlining Your Workflow: Assembly Copy
How to copy in Autodesk Inventor? The Copy command creates a copy or a new instance for selected assembly components. The assembly Copy feature behaves much like Mirror, but is simpler. And yes, Mirror is a method of creating copies (although mirrored). You can read more about mirror here.
After starting the command, select the components to copy in the graphics window or assembly browser. The selected components list in the dialog.
Use the Status to set the action for the components. You can set this on the assembly or to a subset of components. By default Inventor automatically reuses standard content and factory parts.
- Copy creates a duplicate of the component. Each copied component is saved in a new file, which is not associative to the source file.
- Reuse creates an instance of the component, meaning it will change if other instances are changed.
- Exclude does not include the component during the copy operation.
Changing the status of a subcomponent automatically changes the status of the assembly to copy.
With Copy Relationships, Inventor attempts to apply the constraints and joints between the existing components to the copied components. It does not, however, copy relationships to components that are not included in the copy operation. Enable Ground New Components to ground all the new copied components.
After clicking Next, you set the names and locations for the copied components.
You can manually type the display and file names or build templates to automate the naming. Click the plus (+) icon next to either field. This opens a menu of the available attributes that you can insert to build the naming scheme.
You can manually set the file location for the copied components with the User Path option. Or use Source Path to set the location the same as the original components. Use Workspace to set the file location to be the workspace of the active project.
Optionally, enable Create New Assembly to also create a copy of the parent assembly.
During the copy, Inventor maintains the attributes of the source components. This includes relationships, patterns, and representations. However, adaptivity is not recreated. You will need to save the copied component before you can open it in its own window.
Using the Design Assistant to Create Copies
The Inventor Design Assistant is a standalone tool installed with Inventor. Consider it a simple file management tool. Use it to find, track, and manage (rename, revise, replace, and edit properties) files and related documents. It also allows you to copy assemblies to new designs.
Start by opening the highest-level file you want to copy. If it’s an assembly and a drawing you want to copy, open the drawing first. The Design Assistant opens the file and automatically includes all of its references. Tip: Before opening the assembly or drawing, ensure that you set the project.
Then, in the Manage section, use the Action column to set the operation. This includes copy, rename, and replace. So yes, you can create a copy of the assembly and, rather than copying a subcomponent, replace a component with something that already exists.
You can right-click on the File Location cell to access Change Location and copy the file to a different location than the original. You can do this operation with multiple rows selected.
To set the file name of the copied component, right-click on the Name column and pick Change Name. This lets you set the file name AND the destination file location.
With the actions, file locations, and file names set, pick Save to start the copy process.
How to Copy in Autodesk Inventor… Using Vault Copy Design?
Out of scope for this article, but when needing to copy assemblies, especially with more complex assembly structures, doing this manually using Save As, or even the Design Assistant, can quickly become a struggle. If you are using Autodesk Vault, you should consider using Copy Design. This feature is purposely designed for this. It copies the entire design set, including assemblies, sub-components, and the related documentation, all while preserving file integrity. It automatically manages file references, property modifications, and naming standards, starting your project cleanly and exactly.
Anything Else…?
I wrote this article to capture all the ways to copy objects in Inventor. But there are other tools that create copies. Mirroring and patterning are both methods of duplicating geometry. And good news, we’ve already covered these in depth!
Duplicate Your Designs: A Guide to Inventor’s Assembly Mirror
Duplicate Your Designs: A Guide to Patterning in Autodesk Inventor
Duplicate Your Designs: A Guide to Autodesk Inventor Assembly Patterns
And an article I wrote for Autodesk… Duplicate Your Designs: A Guide to Sketch Patterns in Autodesk Inventor
