Skip to end of metadata
Go to start of metadata

You are viewing an old version of this page. View the current version.

Compare with Current View Page History

Version 1 Next »



Part 1: Prepare the Files in Rhino 


Part 2: Fusion360


Step 1: Prepare Files


  • The goal of this section is to create:
    • an STL file that represents our stock
    • an STL that represents the model we want to end up with and cut out on the CNC.
    • a DXF file that represents the perimeter of our model within our stock
  • We will be using Rhino for the following steps.
  • Make sure you are working in inches (if not, type in the units command to change it)
  • You should have a mesh file of the thing you want to cut. It could be an STL file of something you found online, an export from a program like Civil3D, or something you made in Rhino or Sketchup. Any type of file that Rhino can import should work.
  • Drag and drop the mesh file of your model into Rhino and "insert file". Click 'ok'. Then 'ok'. Then 'ok'. Click the origin to place the mesh
  • Move the mesh into its own layer named "model". Hide the layer.
  • Create a new layer named "stock" 
  • Use the Box command and create a box the same size as your stock. Measure the length and width with a tape measurer to the nearest 1/16th inch and the depth to the nearest .001" using digital calipers. 
  • Lock the stock layer so it can't move.
  • Unhide the model layer.
  • Click on your model. See if it says "1 block instance added to selection" in Rhino. If it does, type "explode" and hit enter. If it doesn't say this, don't do this step.
  • Scale your model as needed to make it fit inside your stock. I like to use the Orient command to scale it inside of the stock, however, you can also use the scale command and use the gumball to move the model inside of the stock.
  • If you want to cut out the entire model, follow these steps:
    • draw a rectangle above the stock that is the exact outline of your model
  • If you would only like to cut out a portion of your model, follow these steps:
    • Draw a rectangle that represents the portion of the model you want to cut out
    • Use the extrudeCRV command to extrude the curve so that it goes through the entire model. Make sure Solid=No and DeleteInput=No (we want to preserve the rectangle you made for later)
    • Type in MeshBooleanSplit. Click the model you want to cut and press enter. Click the extrusion you just made and click enter.
    • You can now select and delete the portion of the model outside of the extrusion.
    • You can now delete the extrusion you made, we no longer need it. Please don't delete the original rectangle that we used to make the extrusion.
  • You can now unhide the stock object, and make sure it is locked.
  • Select both the model and perimeter and move them near the origin of the stock, leaving 1" or 2" from the edge (see image)
  • The perimeter curve can be floating above the stock and model as you see in the picture above. I would recommend moving your model in the z-direction so that the top of the model is just below the top of your stock. It is ok if the bottom of the model is not touching the bottom of the stock.
  • Export Files
    • Select only the model. Type "Export" and hit enter. Select the filetype to export as "STL". Save it with the name model.stl
    • Make sure the stock layer is unlocked. Select only the stock. Type "Export" and hit enter. Select the filetype to export as "STL". Save it with the name stock.stl
    • Select only the contour. Type "Export" and hit enter. Select the filetype to export as  "DXF". Save it with the name perimeter.dxf


Step 2: Import files into Fusion 360

Import files into Fusion 360

    • Important: We need to make sure that you are using inches as the default unit.
      • On the top right side of the screen, click on the circle with your initials and click "preferences"
      • A window will appear. On the left-hand side of that window is a number of options. Under Default Units > Design select "in"  for the option "Default units for new design". Do the same thing for Default Units > Manufacture.

      • Select OK.
      • Under the browser, expand "Document Settings and check to see what your units are. If they are not inches, click the edit icon
    • Import the model.stl file. Click "INSERT" > "Insert Mesh". Fusion 360 Will prompt you to navigate to your mesh file. Once you have found it, click Open then OK and you will have a solid representing your model.
    • Import the stock.stl file. Click "INSERT" > "Insert Mesh". Fusion 360 Will prompt you to navigate to your mesh file. Once you have found it, click Open then OK and you will have a solid representing your model.
    • You may find it helpful to rename the meshes under the Browser>Bodies (see below)
    • Import the perimeter.dxf file. Click "INSERT" > "Insert DXF". 
      • Fusion 360 wants you to choose which plane you place the lines on. Select the plane that is located between the X and Y axis (the XY plane, look at the image below). Click the folder icon and navigate to your linework. Make sure you select "inches" under the units dropdown. Click OK to place your linework.
    • Change the appearance of the stock
      • It will be helpful to make the stock mesh clear so that we can see the model underneath.
      • First, near the bottom of the screen, select "Display Settings" and under "Mesh Display" make sure "Face Groups is not checked. This will make sure that the stock will change appearance in the next step.
      • Right-click on the stock under Bodies > Stock and select Appearance.
      • In the window that pops up, search for "clear" and drag and drop "Glass (clear)"  onto your model
      • You should now have something like the following image (two meshes and a contour)


Create toolpaths in Fusion 360

  • If you haven't already done so, /wiki/spaces/SOAdigitech/pages/75237706. A template file is a pre-made set of CNC operations that will work for a given material and tool. We will be importing it into Fusion 360 later in this guide.

  • In this tutorial, I will be using the "Smooth Landscape Topography" file for Wood and a 1/2" ball nose endmill. 

  • Navigate to the Manufacture workspace by clicking on the button in the top left-hand corner and selecting Manufacture

  • Make sure your project units are inches

    • In your browser, check what your units are set to and edit them by clicking the edit icon.

  • Create a Setup

    • A setup is how we tell Fusion 360 what our stock is and where our origin is.

    • Click Setup

    • Tab 1, Setup

      • On the first tab, called "Setup", set Origin to "Selected Point"

      • Make sure "WCS Origin" is selected and blue (see below)
      • Click the bottom-left-back corner of your stock. The original gumball will move here. This step is very important, take a second to make sure the origin is in the same place as the image below. 
      • Important note: What this last step we did means is that the zero height for the z-axis is the bed of the CNC machine, so when you are zeroing the z-axis, you will place the metal plate on the bed of the CNC, not the top of your material. 
      • This also means that the X,Y origin of your stock is the corner closest to the home corner of the CNC. When you jog the bit over to your stock, you will zero the X and Y position to this corner.
      • Lastly, under "Model", select "Nothing". It now wants you to select your model. Since your model is inside your stock, we can't simply select it in the view. We will have to expand the browser and select the mesh directly under Models > Project Name > Bodies > Model. See the image below.


    • Tab 2, Stock
      • On the Mode dropdown, select "From solid" and select your stock. Be careful as to not select your model.
    • Tab 3, Post Process
      • Under "Program Name/Number", give this setup a descriptive name. This will be the name the file saves as later.
    • Hit OK
  • Import template
    • This is the step where we import the template file you downloaded /wiki/spaces/SOAdigitech/pages/75237706.
    • Right-click on your "Setup1" and select "Create from template".
    • A window will appear. On the left-hand side, click My Templates > Local
    • Click the little "Import" icon and navigate to the downloaded template
    • Select the newly loaded template and click the "Select" button.
  • Once you have loaded the template file, you will see a number of operations under your setup, all of which will have a red error symbol.. We will need to go into each operation and update the referenced model, stock, and outline contours to the ones you added in the last section.
  • For Smooth Landscape Topography
    • Operation 1: "Create clearance around part"
      • Double-click on the first operation called "Create clearance around part". A window will pop up.
      • Click the second tab named "Geometry"
      • Click the box that says "Nothing" next to "Contour Selection" and select the perimeter rectangle you imported.
      • Important: Look at your model in the same way as seen in the image below by clicking "front" on the view cube in the top right-hand of the screen. Look for the little red arrow that determines which side of the line the bit will cut on. Click the arrow to change it to the other side. Make sure the little arrow is on the outside of the perimeter contour.
         
      • Click "ok"
    • Operation 2: "Roughing Pass"
      • Double-click on the first operation called "Roughing Pass". A window will pop up.
      • Click the second tab named "Geometry"
      • Click the box that says "Nothing" next to "Machine Boundary" and select the perimeter rectangle you imported.
      • Click the box that says "Nothing" next to "Model Surfaces" and select your model mesh. You may have to expand your project in the browser and find your mesh under "Bodies"
    • Operation 3: "Finishing Parallel"
      • Double-click on the first operation called "Finishing Parallel". A window will pop up.
      • Click the second tab named "Geometry"
      • Click the box that says "Nothing" next to "Machine Boundary" and select the perimeter rectangle you imported.
      • Click the box that says "Nothing" next to "Model Surfaces" and select your model mesh. You may have to expand your project in the browser and find your mesh under "Bodies"
      • Click the box that says "Nothing" next to "Avoid/TouchServices" and select your model mesh again. Make sure that 'Mode' is set to 'touch'
    • Operation 4: " Cut out part"
      • Double-click on the first operation called "Cut out part". A window will pop up.
      • Click the second tab named "Geometry" 
      • Click the box that says "Nothing" next to "Contour Selection" and select the perimeter rectangle you imported.
      • Important: Look at your model from the front by clicking "front" on the view cube in the top right-hand of the screen. Look for the little red arrow that determines which side of the line the bit will cut on. Click the arrow to change it to the other side. Make sure the little arrow is on the outside of the perimeter contour.
      • Click "ok"
  • It may take a few minutes for all of the operations to finish generating. If the process has a percentage next to it, it is still generating


Simulate

  • Now that all of the processes are done generating, we will simulate the whole setup to get an idea of what will happen on the Shopbot CNC.

  • Right-click "Setup1" and select "Simulate"
  • Make sure the checkbox next to "Stock" is checked. This will let us see the stock being removed.
  • Press the play button at the bottom of the screen to start the animation.
  • You can change the speed by dragging the dot on the little slider at the bottom of the screen to the right.
  • I usually speed up the animation a bit and watch to make sure nothing odd happens during the machining operations. 

Post-Process

  • Before you start, make sure you have downloaded this file. Drag and drop it onto your open Fusion 360 window.
  • Once you have simulated your toolpaths, it is time to export the file as a .sbp file that can be read by the Shopbot control software in the Build Lab
  • Right-click on "Setup1" and select "Post Process"
  • The Post Process window will appear.
  • Under the "Post Configuration" section, type in "Shopbot" in the search box and make sure "ShopBot OpenSBP / shopbot" shows up.
  • Select "Post"
  • A dialog box will pop up to save the file.
  • You are now ready to go to the Build Lab and use the ShopBot CNC machine (once you have been trained, of course)
  • No labels

Confluence Documentation | Web Privacy Policy | Web Accessibility