Epilog Laser Cutting With Fusion 360



Posted in TechnologyLasers

Introduction: Epilog Laser Cutting With Fusion 360

About: Instructable newbie, Fusion 360 expert, Mechanical Engineer, and CNC Programmer

If you're anything like me, you love making things. In Autodesk's BUILD Space in Boston, we have four beautiful Epilog laser cutters, yet I haven't been taking advantage of the incredible usefulness of a laser cutter since I am TERRIBLE using both Illustrator and Inkscape, (I know, I should suck it up and learn), but I don't have the same confidence that I do with a milling machine or router.

This is a quick overview of how I have very recently started using the Epilog Laser Cutter with only Fusion 360 and Google Chrome.

Step 1: Create Your Fusion 360 FIle

I would recommend starting in Fusion 360 by going to [Your Name] > Preferences and changing the default modeling orientation to Z-Up. Then create a new design. Making this change first saves a step at the end.

If you want to import an SVG or DXF file, go for it!

If you're creating your model in Fusion like I normally do, great!

If you just want to get the workflow down, make a simple coaster with me.

  1. Make a 3"x3" square on the X-Y plane
  2. Extrude it by 0.25"
  3. Put a 0.5" fillet on the outside corners
  4. Congrats, you're done with your model!

Step 2: Enter the CAM Workspace

Fusion has multiple "Workspaces," each with its own primary function. The default workspace is "Model," but if you're laser cutting, you may want to try "Sheet Metal" as well. With the application of heat, Acrylic can be bent like metal.

To switch workspaces, click the large button at the top right of your Fusion 360 window and select "CAM."

Step 3: New Stock Setup

Creating a new stock setup defines three things in Fusion 360: The orientation of the coordinate system, the location of the origin point, and the size of the material you're cutting.

  1. Click on Setup > New Setup
  2. If you set Z-Up in the preferences and created a new design, the coordinate system should be properly oriented (X-Right, Y-Back, Z-Up). If the orientation of the coordinate system does not match the image, select the stem of the Blue (Z) arrow and select the top face of the coaster.
  3. Set the origin point by first clicking on the white dot at the center of the RGB arrows (Fun fact: this cluster of arrows is called the "Gnomon"). You should see white dots on all corners and edges of the yellow box. Select the left, back, top corner
  4. In the new setup dialog box, select the stock tab. In the Mode Dropdown, select Fixed Size Box. If you're doing a coaster with me, set your dimensions to 3in by 3in (X&Y) and 0.25in thick (Z). If you're using your own design, make these dimensions roughly the size of your material. You may want to play around with Model Position ("Offset from back" and "Offset from left") as well.
  5. Click OK

Step 4: Apply Your Toolpath

  1. Click on the 2D Profile button in the Cutting menu.
  2. Select a tool by clicking on the select button. I picked the .015" laser cutter, but actual kerf (cut) width depends on the power and focus of the laser cutter. You can find an Instructable on measuring kerf width here.
  3. Select the top edge of the coaster. This should automatically move you from the Tool to the Geometry tab. While you're in the Geometry tab, decide how you want your tabs spaced, or if you want them at all. For this tile, I'll uncheck the box next to Tabs.
  4. Switch to the Passes tab and set the Sideways Compensation to "Center"
  5. Lastly, switch to the Linking tab. You probably don't need it, so un-check Lean-In (Entry) and Lead-Out (Exit), and set Pierce Clearance to 0

Step 5: Post Your File

Now We're ready to post-process your toolpath. Before you do, you'll need to download the Epilog post-processor from the Autodesk Post Library. ( Link)

  1. With your toolpath selected, click the post-process button in the toolbar
  2. Click Setup, then Open Folder. Copy the downloaded file into this folder.
  3. Click Cancel in the Post Process dialog box and re-open the Post-Process dialog box
  4. In the Post Configuration dropdown menu, select epiloglaser.cps
  5. In the properties tab, set (Built-in) minimumCircularRadius to a value 100 or higher. The way that arcs and circles are created doesn't translate well to the Epilog control, so this will break your arcs and circles into very small lines.
  6. Optional: Set the (Built-in) Tolerance between 0.005 and 0.02. This is the primary factor in the post determining how many lines it needs to break your curves into. A larger value will leave a rougher curve but will cut faster.
  7. Check the box next to "Open NC file in editor"
  8. Click OK
  9. Pick the save location (I over-write the same file over and over)
  10. Click OK

If your computer just opened a Google Chrome page, proceed to the next step. If not, try this step over.

Step 6: Print Your File

  1. In Chrome, click File > Print (or Ctrl+P)
  2. Set your margins to 0 or None
  3. Click Print using system dialog
  4. Select your Epilog and click Printer Properties
  5. At this point, you should see the same dialog box that you're familiar seeing with the Epilog. Set your power, speed, and frequency (I use 7s, 100p, 100f for 1/4" acrylic), and click Apply, then Print.

Your cutting job should now be loaded into the Epilog. From this point forward, follow standard operating procedures for your Epilog Laser.

Step 7: Have Fun!

As I learn more about this process, I'll continue to update this Instructable. I'm currently exploring the best workflow for Rastering and etching using color mapping. In a nutshell, you can define red as a vector cut, green as etch/raster. Fun fact: Goldfinger uses a red laser since he's trying to vector cut James Bond in half. XD

Happy laser cutting!



    • Spotless Contest

      Spotless Contest
    • Microcontroller Contest

      Microcontroller Contest
    • Space Challenge

      Space Challenge

    We have a be nice policy.
    Please be positive and constructive.