CNC Cut Files with Autodesk Product Design Suites, Part 1


This handout was written as a supplement to the Autodesk University 2013 class given by Scott Moyse and Gavin Bath. They were kind enough to permit it to be formatted in two parts and published here. Some of the information was covered in more or less detail to suit that limited class format.

Part 1 will begin coverage of the various methods of producing 2D CNC cut files or tool paths within Autodesk Inventor®.

In an upcoming issue, Part 2 will discuss using iPropWiz to configure your Inventor design environment and benefit you in the long run. We will also introduce the concept of using Autodesk® Vault to manage your design data, and ultimately your manufacturing data, as well as some methods of presenting that to CAM programmers and staff on the shop floor.



2D CNC Cut Files

   Flat Pattern Export
   Flat Pattern Export Add-In Example
   Export Face
   Export Sketch As
   Create a Drawing
   Setting up a Sketch Text Style


2D CNC Cut Files

I know of five distinct ways to get what CNC programmers need out of Inventor. The best method for you depends entirely on what you are cutting and the software you are using to program it. In the past I’ve had to resort to some fairly lengthy procedures to get what was needed. With building or yacht interiors, the difficulty comes in dealing with the grain direction of the veneers or laminates on parts and subsequent grain matching. As a result I have investigated lots of options and discovered a few tricks along the way.

Flat Pattern Export

As you may well know, in an Inventor sheet metal part you can create flat patterns. Once a flat pattern has been created, you can save out a dwg/dxf to AutoCAD®, which will allow you to develop the cut file further if need be.

Figure 1: Layer mapping options for flat pattern export

Figure 2: Geometry clean up settings for flat pattern export

There is some scope to run a macro in AutoCAD to do some clever post-processing on the flat patterns to streamline the CAD to CAM process. For a lot of people this would mean getting the part number into the cut file.

Figure 3: The result of a flat pattern export automates the assignment of layers for some of the model features


  • Merge profiles into closed polylines.
  • Spline conversion to polylines.
  • Object recognition: inside and outside, and features on the upper and lower faces.
  • Rebase geometry to 1st quadrant.
  • To a certain extent, ability to control the layers.
  • Semi-automated length, width, and thickness values for BOM and parts lists.


  • No support for exporting text with the cut file/flat pattern!
  • No feature recognition, so there’s no method to include feature depths in the 2D data.
  • The process has to be carried out manually on each part, so it’s the same repetitive process over and over again.
  • Sheet metal thickness won’t link through to body extrusion value easily when using multi-body modeling techniques.

Flat Pattern Export Add-In Example

Here is an example of how automating Inventor can make the process of creating sheet metal flat patterns a breeze.

Figure 4: Export assembly flat pattern

For many companies, the creation of 2D data for profile cutting can be a hugely repetitive, manual task that costs significant time. We tend to find that the requirements for exactly how the data is presented varies a lot. For this reason, it's difficult to come up with a "one size fits all" approach for automating this task. This particular example is for a manufacturer who requires a table of information in a cut kit as well as 2D DWG files for each component. The tool runs as an Inventor add-in and works in the assembly environment.

With an assembly file loaded, the command is executed and the routine runs through every sheet metal component in the assembly, creates its flat pattern (if it doesn't already exist), and then exports the flat pattern as a DWG.

Figure 5: Flat patterns created automatically for all sheet-metal components

Once the flat patterns have been created, an email is automatically generated with a HTML table that contains thumbnail images of each component as well as dimensional information, material, and assembly quantities. Additionally, the DWGs are attached.

Figure 6: Example email generated by tool

This customization can be very easily edited to manipulate the data that is output; for example, changing from DWG to DXF file format.


  • Provides confidence in accuracy of quantities and dimensional information.
  • Really fast and very efficient.
  • Email trail provides job ordering history.
  • Not easy to fudge quantities, add spares, etc. without modifying assembly.


  • Not easy to override quantities, add spares, etc. without modifying assembly.
  • Reliance on programmer to edit customization if requirements change.
  • Doesn't handle non-sheet metal parts (unless identified somehow).
  • Doesn’t handle grain direction on grain-sensitive materials.

Export Face

Figure 7: Export face radial menu command

I have a couple of videos showing you how to export a face of your part and a sketch in your part as a dxf/dwg file. People often use it for its simplicity—you can quickly knock up a 2D cut file and fire it off to your CAM programmer.

Figure 8: Export face captures the face outline nicely, but it’s missing a lot of 'manufacturing' information

Export Face Pros:

  • It’s quick and simple.
  • There are some AutoCAD export options for objects and file type.
  • The result is closed polylines.

Export Face Cons:

  • Zero layer mapping options like there are in the flat pattern tool.
  • It doesn’t capture geometry of the entire part, such as rebates, bevels, and hidden features, etc.
  • No ability to include text in the export for engraving.
  • No ability to color the features by type for export.

Export Sketch As

Figure 9: Export Sketch As allows you to capture additional information which can be added to the sketch

Export Sketch Pros:

  • Quick and simple process.
  • Some AutoCAD export options for objects and file type.
  • The sketch tools allow you to project geometry not included in the Face export.
  • Resulting geometry made up of closed polylines.

Export Sketch Cons:

  • Zero layer mapping options unlike the flat pattern export tool.
  • No ability to export text for engraving.
  • No ability to color the features by type for export.

To clarify the engraving text issue, in both situations above you could emboss the text and have it exported with the face or sketch. However, this results in a text outline instead of a text center line. This is very inefficient for CNC machines to cut when the number is only there for practical rather than aesthetic reasons.

Create a Drawing

Figure 10: Inventor part with associative sketch cut file

This is my preferred method of generating cut files if you have a requirement for engraving or etching text onto your parts.

The two reasons for wanting to create cut files using the drawing environment are:

1. 2D labeled cut files saved in a single file. In this case you may want to:

a. Group your 2D cut files by material and thickness.
b. Then use leaders or balloons to access and display your parts iProperties.
c. Add instructions to the individual views via icons/symbols or notes for the CAM Programmer(s).

2. 2D cut files via model sketches:

a. Group your 2D cut files by material and thickness.
b. Display colored model sketches instead of visible edges.
c. Display positioned sketch text for CNC engraving.

I’ll focus on the second option here:

  1. Create your part.
  2. Add a sketch for any projected geometry (reference geometry).
  3. Add a sketch for ‘sketched’ geometry and sketch text.
  4. Look at the top face (the one with the sketches on it) and set the view cube view as Front. This step is optional, but helps placement of the part views later.
  5. “Rinse and repeat” for the other parts.
  6. Create a drawing.
  7. Start placing views, making sure the views are perfectly normal to the sketch faces.
  8. Right click on each view in the browser and select ‘Get Model Sketches.’
  9. Check that all sketches are visible (sketches containing reference geometry won’t be visible if they contain ‘sketched’ geometry as well).
  10. Turn off the Visible Edges layer (to reduce/remove duplicate geometry).
  11. Save as AutoCAD DWG.
  12. In AutoCAD use Quick Select to select geometries by color and add to the appropriate layer.
  13. Use the Overkill command to clean up the geometry.
  14. Close polylines using the polyline edit command and the multiple option.
  15. Check that all the cut files are “water tight” and open only where intended.

Following that workflow alone would get you there. However, if you use Inventor DWGs as your company’s standard drawing file format, then the following video demonstrating the use of the ‘EXPORTLAYOUT’ command in AutoCAD, may result in a few less files for you. Thanks to Paul Munford for letting me know about this one:

So you may be thinking what a mission it is creating all this lot, however, you can automate the process via an add-in or a macro. So I thought I would share a video of one of our cut file macros at work:

What really gets me excited about this workflow is its associativity with the base files. You can do the hard work of creating your CNC cut files while the product is still being designed. Any subtle changes which occur prior to the design being released for construction are associatively updated. All, with very little effort and at the click of a button, are exported en masse to a dxf/dwg for some pre=CAM prep.

Figure 11: Once exported to DXF/DWG, the txt font becomes centerline text


  • Associative cut files.
  • Allows you to manage exactly what geometries you want in the cut file.
  • Export of the ‘txt’ font text results in center line text in AutoCAD, which is perfect for CNC machines.
  • Geometry layers and color settings are maintained on Export which can then be leveraged efficiently in AutoCAD.
  • Batch processing of cut files is possible natively, with zero customization.
  • The result is a single file containing multiple cut files which allows for efficient preparation in AutoCAD prior to CAM import


  • Resulting geometries are individual and open.
  • Splines aren’t converted to polylines.
  • Based on the listed workflow, all geometries are on the same layer.
  • The result is a single file containing multiple cut files which can mean a lot of work splitting up the cut files in the CAM software prior to nesting.

Setting up a Sketch Text Style

Figure 12: Sick of changing these settings all the time?

Do you find yourself swearing at Inventor when you have to repetitively set the font, size, and color of your sketch text in the part environment? It used to really irritate me that the dialog was identical to the one in the drawing environment, but the text style drop-down is permanently greyed out and set to ‘Default ANSI’ or ‘Default ISO’ depending on your default standard. I just wanted to pick my own style, which had the presets I use most often and couldn’t. But there is a sneaky undocumented workaround.

If you were to look in the styles and within all the Inventor folders on your local drive for any trace of a text style named ‘Default ANSI’ or ‘Default ISO,’ etc., you won’t find anything. So the trick is to create a text style matching the exact name of the style you can’t find, then just configure it with the settings you are so fed up with selecting each time you create a new text box.

Figure 13: Create a new text style with an identical name as the ‘greyed out’ text style in the text editor

The next time you create a text box in a sketch, all of your settings will be just so. If you’ve been creating a ton of CNC cut files requiring text engraving with Inventor, it’s at this point you may weep a little (I certainly did).

Figure 14: Check that out! Perfect settings every time

Thanks to the individual who shared this solution with me a number of years ago via the Autodesk Discussion Forums.


Thank you to Gavin Bath for contributing a huge effort towards this article, and also CADPRO Systems Ltd. for allowing this information to be shared publicly.

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