CNC Router CAM Training

Step 0 — Open and modify model

  • Open the model in Fusion360
    • In this Guide, we’ll be working with “Shopbot Nameplate”
  • Make sure you are in ‘Design’ mode
  • You can modify the text by right clicking on it and selecting “Edit Sketch” which will open “Sketch2”
    • Now doubleclick the text to change it to what you want
    • When you are done editing the text click “FINISH SKETCH” to return to the main view
  • You can modify the shapes as well, but do not change the overall outline of the model
    • Highlight a shape by clicking the corner above it and dragging over the shape
    • Use keyboard shortcut ‘m’ to give yourself arrows that you can use to move them around
    • Hit delete to delete a highlighted shape

Step 1 — Set up your model in the Manufacturing workspace

  • If in the Model workspace, change to Manufacture by clicking on the “Model” dropdown in the top left corner of your screen

Step 2 — Create a new setup

  • To begin your setup, select the “Setup” dropdown in the upper left hand corner, and click on “New Setup”

Step 2a — Setup your Stockbox

  • Click on the “Stock” tab to setup your stockbox to match your actual stock size
  • Select the dropdown menu next to “Mode” and choose the mode that works best for your project
    • For the nameplate, we will be working in “Fixed size box” mode
  • Enter the width, depth, and height of your stock
    • For this training, use stock dimensions of 10 in x 5 in x 0.5 in which will be for a sheet of plywood
    • NOTE: During the training session we will measure the actual height of the stock and update the height value accordingly

Step 2b — Specify your datum point

  • Click on the “Setup” tab to setup your coordinate system
  • Under the Work Coordinate System (WCS) field set the “Orientation” to “Model orientation”
    • NOTE: The direction of the axes in your setup orientation need to match the direction of the Shopbot axes of motion
  • Select your datum point (the origin of your part the machine will reference)
    • First change your mode of selection by choosing the dropdown next to “Origin” and selecting “Model box point” mode
  • Select the box next to “Model Point” which says “Box Point”, then select the point at the left, front, top of your model as your datum point
    • The axis marker should now move to this point
  • Click “OK” at the bottom of the setup menu
  • NOTE: Fusion automatically displays a generic router in the background once you make a setup. To hide this object, go to your Browser and open up “Setups > Setup1” which should show “Autodesk Generic 3-axis” which you can hide by clicking on the eye symbol next to it.

Step 3 — Begin your toolpaths with an Engraving toolpath

  • The first toolpath we will create is to engrave the writing on the face of your nameplate
  • Click the “2D” dropdown menu and select the “Engrave” toolpath

Step 3a — Engraving: Select tool

  • The first step to creating any toolpath is selecting your tool. We will be building all of the tools for our program from scratch.
  • To open the tool library, click on the “Select” button next to the “Tool” option

Step 3b — Engraving: Select chamfer tool

  • We will build a tool library that is specific to the tools we will be using for this part. Some shops have tool libraries that you can download.
  • First we will add a 1/2″ 45 degree chamfer bit
    • Click on the “+” symbol in the top left hand corner of the center area
    • Under the “Milling” heading select “Engrave/Chamfer mill”
    • This will open a new tool window
  • Set each of the following parameters
    • General
      • Description: “.500″ x 45 Chamfer Tool”
    • Cutter
      • Type: “Engrave/Chamfer mill”
      • Unit: “Inches”
      • Clockwise spindle rotation: checked
      • Number of flutes: 2
      • Geometry
        • Diameter: 0.5 in
        • Shaft diameter: 0.25 in
        • Tip diameter: 0.03 in
        • Overall length: 2 in
        • Length below holder: 0.5 in
        • Shoulder length: 0.5 in
        • Flute length: 0.25 in
        • Taper angle 45 degrees
    • Post processor
      • Number: 2
  • Click “Accept”
  • Click “Select” in the bottom right corner to finish selecting the chamfer tool for the engraving toolpath

Step 3c — Engraving: Set tool parameters

  • Under the “Tool” tab go to “Feed & Speed” section
  • Select the dropdown next to the “Preset” parameters and select “Custom”
  • For the chamfer bit we will use the following settings
    • Spindle speed: 18000 RPM
    • Cutting Feedrate: 130 in/min
    • Lead-In Feedrate: 65 in/min (Lead-in feed should be half of feed)
    • Lead-out Feedrate: 65 in/min
    • Ramp Feedrate: 65 in/min
    • Plunge Feedrate: 43.33 in/min (should be about 1/3 of cutting feedrate)
    • NOTE: The “Feed per Tooth” should automatically change to “.003611 in”

Step 3d — Engraving: Contour Selection

  • Click the “Geometry” tab in the engrave toolpath window
  • Next to the “Contour selection” parameter select the button with the text “Nothing”
  • Select your text, after which it should be highlighted blue
  • Click “OK” to complete the build of your first toolpath

Step 4 — Create a 2D Pocket toolpath for the shapes

  • The next step is to create the toolpath for the shapes on the face of your stock
  • Click the “2D” dropdown menu and select the “2D Pocket” toolpath

Step 4a — 2D Pocket: Select tool

  • Open the tool library by clicking on the “Select” button next to the “Tool” option.

Step 4b — 2D Pocket: Select flat endmill

  • For the “2D Pocket” operation to cutout the shapes and the “2D Contour” operation to cutout the whole part we use a “1/4 in Flat Endmill”
  • To do this we are going to repeat step 3b but for a different bit
    • Click on the “+” symbol in the top left hand corner of the center area
    • Under the “Milling” heading select “Flat end mill”
    • This will open a new tool window
  • Set each of the following parameters
    • General
      • Description: 1/4″ Flat Endmill
    • Cutter
      • Type: Flat end mill
      • Unit: Inches
      • Clockwise spindle rotation: checked
      • Number of flutes: 3
    • Geometry
      • Diameter: 0.25 in
      • Overall length: 2.5 in
      • Length below holder: 0.85 in
      • Shoulder length: 0.75 in
      • Flute length: 0.75 in
    • Post processor
      • Number: 1
  • Click “Accept”
  • Click “Select” in the bottom right corner to finish selecting the flat endmill tool for the pocket toolpath

Step 4c — 2D Pocket: Set tool parameters

  • Under the “Tool” tab go to “Feed & Speed” section
  • Select the dropdown next to the “Preset” parameters and select “Custom”
  • For the flat endmill bit we will use the following settings
    • Spindle speed: 11,000 RPM
    • Cutting Feedrate: 130 in/min
    • Lead-In Feedrate: 65 in/min (Lead-in feed should be half of feed)
    • Lead-out Feedrate: 65 in/min
    • Ramp Feedrate: 65 in/min
    • Plunge Feedrate: 43.33 in/min (should be about 1/3 of cutting feedrate)
    • NOTE: We are aiming for a “Feed per Tooth” of ~.004 in

Step 4d — 2D Pocket: select geometry

  • Go to the “Geometry” tab (second tab)
  • Next to the “Pocket Selections” parameters select the button with the text “Nothing”
  • Select the bottoms of the pockets
  • IMPORTANT: Make sure you select the bottoms of the pockets, if you select the tops, you have to adjust the height later

Step 4e — 2D Pocket: set Multiple Depths

  • Go to the “Passes” tab (fourth tab)
  • Check the “Multiple Depths” field
    • Set the “Maximum Roughing Stepdown” parameter to “.125 in”
  • Unselect the “Stock to Leave” field

Step 4f — 2D Pocket: set Linking Parameters

  • Go to the “Linking” tab (fifth tab)
    • Linking parameters are where we adjust how individual parts of a toolpath are connected to each other
  • Under the “Ramp” field set the “Ramp Type” to “Plunge”
  • Click “OK”

Step 5 — Create a 2D Contour toolpath to cutout the nameplate

  • The final toolpath to create is to cutout your entire nameplate from the stock
  • Click the “2D” dropdown menu and select the “2D Contour” toolpath
  • NOTE: We do not have to select a tool or change the “Feed & Speed” for this toolpath as we will be using the same values as we did for the “2D Pocket” toolpath

Step 5a — 2D Contour: select geometry

  • Go to the “Geometry” tab (second tab)
  • Next to the “Contour Selection” parameter click the button with the text “Nothing”
  • Select the bottom contour which outlines the entire part

Step 5b — 2D Contour: Add tabs

  • Select the “Tabs” field and set the following parameters
    • Tab shape: Triangular
    • Tab width: .25 in
    • Tab height: .125 in
    • Tab distance: 4 in

Step 5c — 2D Contour: Set stepdown in multiple depths

  • Go to the “Passes” tab (fourth tab)
  • Check the “Multiple Depths” field
    • Set the “Maximum Roughing Stepdown” parameter to “.125 in”
  • Uncheck the “Stock to Leave” field
  • Click “OK”

Step 5d — Adjust bottom height offset

  • Go to the “Heights” tab (third tab)
  • Under the “Bottom Height” field change the “Offset” to “-.020 in”
    • We have to do this to ensure the router will cut all the way through our stock during the contour operation

Step 6 – Simulate

  • Before we export our part we are going to simulate the toolpaths which allows us to
    • Check for crashes
    • Make sure we selected everything we want cut
    • Understand how the tool with perform each operation
  • Open the “ACTIONS” dropdown and click “Simulate”
  • Before we look at the simulation we are going to hide some objects to make the simulation easier to see
    • Under the “Tool” field change the “Tool” parameter to “Shaft”
      • This will make it so we will only see the bit and not the holder
    • Uncheck the “Machine” field
      • This will make the default router machine in the background disappear
  • Now run the simulation by pressing the play button at the bottom center of the window
    • Check to make sure all the operations look good (compare to the example video below)
    • NOTE: You can change the speed of the simulation using the slider under the play button
  • If you see any issues in the simulation go back and fix them
  • Once everything looks good, click on the “Statistics” tab in the “Simulate” window
    • Check the “Machining time” is reasonable (for this nameplate the machining time should only be a minute or so)

Step 7 – Post process

  • The last step is to use a post processor to take our CAM and turn it into G-code
    • Different machines speak different dialects of g-code, so we need to first choose the right post-processor
  • Open on the “ACTIONS” dropdown and click “Post Process”

Step 7a — Search post processor library

  • Select the dropdown next to the “Post” parameter and select “Choose from library…”

Step 7b — Select “ShopBot OpenSBP”

  • Type “SBP” in the search bar in the top left to search post processors for ‘SBP’ (ShopBot Post)
  • Click the “ShopBot OpenSBP” post processor
  • Click “Select”

Step 7c — Post file

  • The Program Name/Number must be a number–traditionally 5 digits. A good practice is to have parts that have multiple setups have related numbers. For example, the nameplate has 3 operations. They could be numbered 11111, 11112, and 11113 to show that they are related to each other.
  • Change the “File name” to “kerberos_CNC_Router_Training” where you should substitute “kerberos” with your own
  • The “Program Comment” is what will show up as the name of the program. This should be descriptive of the part and which operation this setup is. The nameplate can be “Nameplate Op1”.
  • You can also change the “Output folder” to a different location
  • Hit “Post”!

Step 8 — Complete

  • Save your G-code file to a flashdrive and bring it with you to the training

Related Articles

Responses

This site uses Akismet to reduce spam. Learn how your comment data is processed.