Steps to a Machining Project

0. Get added to Bechtel Fusion Team

  • Only the Front Desk can add you to the Fusion Team! So please get in touch with them.
  • Enable Cloud Libraries
  • Steps of Fusion Team
  • Fusion Team Troubleshooting
  • 1. Idea Generation and Design

    2. Optimization for Manufacture

    • UNITS: Machines at the Bechtel Center are Imperial, please use inches, not millimeters
    • Remove or modify features that make manufacturing more difficult
      • Ex: Remove unnecessary fillets, add a relief hole to the apex of a sharp inside corner so that it is manufacturable
    • Change arbitrary features to common sizes
      • Ex: make an arbitrary hole 0.250” instead of 0.283”
        • Highest performance tooling is only available in common sizes
          • Other sizes are available only if necessary
    • Avoid features that are too deep for tooling to reach
      • Small diameter holes or slots that are very deep
      • No hollowing out blocks when flat material could be welded to shape
    • Minimize features that stick up unsupported, like fins or standoffs

    3. Model the stock that contains your part

    1. Model the stock (raw material)
      • Pro-Tip: If you don’t know what your stock size is going to be, you can use parameters [Modify] -> [Edit Parameters] -> [User Parameters +] to make variables that can be quickly edited when you’re at the center
      • Add 0.25in of extra material to the front of lathe stock to add clearance for facing passes
    2. Use [Assemble] -> [New Component] -> [From Bodies] and select to change your part and then your stock into two separate components
    3. Use [Assemble] -> [Joint] and select the top center of your part and stock to join them together, flipping if necessary
      • Include a small offset from the top of your stock
      • Hold {Ctrl} while selecting the reference points to enable Fusion’s snap functionality, it’s great
    4. Right Click on your stock component in the project tree and [Change Opacity] for easier use
    Part within Stock, both as components, joined together

    4. Programming and Toolpath Generation

    Mill:

    1. Import the machine table to be used into the model
      1. In the data panel (9 dots in the top left), navigate to the [Workholding and Stocks] project, go into the [Tables] folder, find the table of the machine you would like to use, and drag and drop it into your project
        • DO NOT EDIT THE TABLE MODEL IN THE WORKHOLDING REFERENCE FOLDER!
      2. Right click on the machine table in the object tree in the top left, select [Break Link]
        • You can press {Shift+N} to enable colors!
      3. Create a new joint to place your stock centered between the vise jaws at the specified point
        • If you need to change the vise on the table model, delete the existing one in the model tree and repeat steps 1-3 to place the correct vise in the same position. See our Workholding Guide
      4. Under [Modify] use [Change Parameters] to edit the jaw gap of the desired vise to hold your stock
        • NOTE: You cannot cut below the vise jaws, if your part has features that go to the bottom, raise the part by offsetting the joint between it and the vise but the more material the vise holds, the better
    2. Setup the CAM Program
      1. Switch to the manufacture tab and click [Setup]. Select your part as the model, then check the [Fixture] box and select the table model and workholding.
      2. Select whichever machine you will be using, according to the table model you have selected
      3. In the [Stock] tab, the [Mode] dropdown select [From Solid] and select the stock component.
      4. In Setup, the Work Coordinate System with the X-axis right, Z-axis up as shown. Follow the red arrow to set the [WCS Origin] -> [Selected Point] to the center of the bolt we have in the machine
    3. Create Toolpaths
      1. Right-click on the setup in the browser and select [Create from Template].
      2. First, do a probing cycle, select the x and y or z faces of the stock
      3. Under [Actions] in both Probing operations, select [Override Driving WCS] and set it to 2
      4. Select the geometry you wish to probe
        •  Fusion sometimes thinks the probing cycle will crash, usually it’s fine but ask a Peer Mentor about it
      5. Follow the Milling Toolpath Guide to create each of the toolpaths you will be using
        • Each tool can do different materials, if you do not know what material class your part is, check here
        • TIP: Use the largest, stubbiest tool that allows you to cut the geometry
        • Ask a Peer Mentor if you need a tool that is not in the library
      6. Simulate the toolpaths and make sure there no collisions during cutting operations
      7. Have a Peer Mentor look over and approve your setup and program
    Example of a good Mill CAM Simulation with toolpaths shown

    Lathe

    1. Import the Lathe Chuck to be used into the model
      1. In the data panel (9 dots in the top left), navigate to the [Workholding and Stocks] project, find the chuck of the machine you would like to use, drag and drop it into your project
      2. Right click on the chuck in the object tree in the top left, select [Break Link]
      3. Create a new joint to place your stock between the chuck jaws at the specified point
      4. Under [Modify] use [Change Parameters] to edit the chuck diameter to hold your stock
    Part in the ST-20 Collet Chuck
    1. Setup CAM Program
      1. Switch to Manufacture Tab, click [Setup]
      2. Select whichever machine you will be using, according to the table model you have selected
      3. Under [Operation Type], select [Turning or mill/turn]
      4. Select the ST-20 or ST-20Y in the machine model, corresponding to the chuck you’re using
      5. Under Model, select your part then Check [Spun Profile]
      6. Work Coordinate System – select [Z axis], ensure it points out the front of your part, flip the other axes if necessary to ensure the Y axis is pointing up
      7. Origin – [Selected Point] and select the center point for WCS #2
      8. Switch to [Stock] tab, set [Mode] to [From Solid] – select your modeled stock
      9. Back to [Setup] tab, set [Chuck Reference] to [From Solid], select the chuck
    2. Create Toolpaths
    1. Follow the Lathe Toolpath Guide to create each operation, simply select the tools to be used and the geometry that operation will cut
      • Tool information is within the tool library under the Info tab on the right side
      • TIP: Use the stubbiest tool that allows you to cut the geometry
    2. Simulate the toolpaths and make sure there no collisions during cutting operations
    3. Have a Peer Mentor look over and approve your setup and program
    Example of a good Lathe CAM Simulation with toolpaths shown

    5. Peer Mentor Review & Reserve time at the Bechtel Center on the machine to be used

    • See Project Workflow for project review, modification, and approval
    • Reserve at least an hour more than your program’s run time
    • Arrive on time, reservations are canceled after 15 minutes of no-show
      • Teams can only reserve one machine at a time. Anyone operating a machine is required to be familiar with what operations are taking place, (no handing off for others to babysit your program)

    6. Post Process the Program

    • In Fusion, hit the [Post Process] button. Press [Setup] at the top then select [My Cloud Posts]. Under the [Post Configuration], select the BIDC post processor to be used (lathe, mill, gantry).
    • In the [Program Settings] select a UNIQUE 5-digit number (NOT: 12345, 54321, 11111, etc.) and remember it. Add a [Program Comment] of your project with [01] at the end, for version tracking.
    • Save the file to your computer, location is the [Output Folder]
    • Upload your program to the Bechtel Center File Share: