Introduction: Pier 9 Resource: CAD and CAM in Fusion 360 for Shopbot
This Instructable is for workshop users at Pier 9, or anyone who wants to learn:
-CAD (Computer Aided Design) in Fusion 360--creating a solid model with sketches
-CAM (Computer Aided Manufacturing) in Fusion 360--creating simple 2D Pocket and Contour toolpaths
-CNC machining on a Shopbot
This Instructable does not assume any previous experience with Fusion 360 or CNC machining, and is a great first project for beginners. You will model a simple pushstick--a tool for pushing material safely through a table saw--in Fusion 360. You will learn how to use vector drawing tools with dimensions and constraints to create simple 2D profiles that will then be extruded into a solid model. Once you've built the model, you will learn how to create toolpaths to machine the pushstick on a Shopbot CNC router.
If you want to machine the pushstick at Pier 9, you'll need to take:
If you are excited about CNC after finishing this project, you can continue building your skills with the following courses at Pier 9:
Let's get started! All you'll need is your laptop, an Internet connection, a three-button mouse, and a USB flash drive.
Step 1: Download Fusion 360
Step 2: Create New Project
1) Open Fusion 360.
2) In the data panel on the left side, click New Project at the top. Name it "Shopbot push stick" and press Enter.
3) The new project should still be highlighted in the Data Panel. Double click it to open it.
4) Click the "ice cube tray"--the button with nine squares on it--to close the Data Panel and free up screen space.
5) Explore the view cube in the top right corner.
You can click on the cube's faces, edges, and corners to rotate your view. Clicking the "home" icon that appears when you hover your mouse over the view cube returns you to your original orientation.
6) Practice navigating with your mouse.
Pan: Hold down scroll wheel
Zoom: Scroll with the scroll wheel
Orbit: Hold down shift, hold down scroll wheel
Step 3: Create Sketch
1) Click the dropdown in the top left corner to change the current Workspace to Model.
This is the workspace that is best for creating simple prismatic (2D features at different depths) models.
2) Under the browser on the left side of the screen, click the icon next to Units. In the dropdown, change Units to inches and click OK.
3) In the ribbon at the top, click the Sketch dropdown and click Create Sketch.
4) Click the XY plane, or the plane that aligns with the red and green arrows.
The view will re-orient so that you're directly facing the sketch with an orthographic Front view.
It's important to understand that CNC locations are dictated by Cartesian coordinates, ie, three number lines called X, Y, and Z, that are perpendicular to one another.
In Fusion 360, red = X, green = Y, and blue = Z.
If you're not familiar with the CNC Right Hand Rule, this is a useful way of remembering the positive direction of each axis. When you are facing a CNC machine, put your right hand out, palm up, and extend your thumb, index finger, and middle finger, as indicated in the diagram. Your thumb points in +X, index finger in +Y, and middle finger in +Z.
When drawing and extruding sketches to create a model that you're planning to machine, it's useful to draw all sketches on the XY plane. This way, you will extrude them along the Z (up and down) axis and they will be set up correctly when it comes time to generate toolpaths.
Step 4: Draw Triangle
1) In the ribbon at the top of the screen, choose Sketch>Line.
Alternatively, use the hotkey L.
2) First click on the origin, then two more points, and then back to the origin to create a right triangle. The dimensions do not matter right now. The triangle will fill in with a light pink color once it is closed.
In the Sketch Palette on the right, make sure Grid and Snap are checked. This will make your drawing more accurate.
Step 5: Add Dimensions to Triangle
1) Right click on the screen, choose Sketch, and Click Create Dimensions.
Alternatively, use hotkey D.
2) Click the bottom leg of the triangle and drag down. Click to set the field for the dimension value, type 13, and hit Enter on the keyboard. The bottom leg is now 13".
3) Repeat this process to change the dimension of the vertical leg of the triangle to 10".
Step 6: Add Step on Bottom Leg of Triangle
1) In the ribbon, choose Sketch>Line. Or type hotkey L.
2) Draw a short vertical line that snaps to the bottom leg of the triangle, and a horizontal line that snaps to the hypotenuse of the triangle, to create a "step" on the bottom edge of the triangle.
Step 7: Add Dimensions to Step
1) Type D to add dimensions to the line.
2) Click the origin and the bottom point of the new vertical line, and set the dimension to 2.5.
3) Set the dimension of the vertical line to 0.5.
Step 8: Trim Area Around Step
1) In the ribbon, under Sketch, choose Trim.
Alternatively, use hotkey T.
2) Click the two lines that you want to trim away to create a "step" in the bottom of the triangle.
Notice that the line turns red before you trim it.
3) Above the ribbon, click the disk icon to save your part. Give it a name, and save it inside the Shopbot push stick project.
Step 9: Add Fillet
1) In the ribbon, under Sketch, choose Fillet.
2) Click the vertical leg and the hypotenuse of the triangle.
3) Enter a dimension of 3 and hit Enter.
Step 10: Add Center Circle
1) In the ribbon, under Sketch, choose Circle>Center Diameter Circle.
Alternatively, use hotkey C.
2) Click the center point of the fillet you just created.
3) Before clicking again, expand the circle and type 4. The circle will adjust to a diameter of 4". Then click Enter.
Step 11: How to Edit Dimensions
If you created a piece of sketch geometry with rough or incorrect dimensions, Fusion 360 makes it easy to edit dimensions.
1. Enter hotkey D for Dimension Mode.
2. Double click the circle diameter dimension.
3. Re-enter 4 and hit Enter.
Step 12: Add 3-Point Arc
1) In the ribbon, under Sketch, choose Arc>3-Point Arc.
2) Approximately 1" from the far right corner of the triangle, click the hypotenuse, the bottom leg, and the middle of the arc, in that order. Use screenshots as a reference.
3) To exit any drawing mode, right click on the view window, and choose OK. This exits Arc mode.
4) Notice you can now drag and drop the nodes of the Arc to edit its shape.
Step 13: Add Tangent Constraint
It's important to constrain your drawings to keep them clean, organized, and easily editable. Sometimes this happens as you draw. For instance, you automatically created a perpendicular constraint when you drew the initial triangle because you snapped to the grid.
When you drew the arc, it is likely that Fusion 360 automatically created a coincident constraint--meaning that the arc is coincident to the triangle (they share a common point). Zoom into the arc and look at the small white icons that appear at its top and bottom. You can always match these icons to their names in the Sketch Palette.
Fusion 360 may have already created a tangent constraint for you. Look for the tangent icon near the top of the arc. If you do not see it, proceed to the instructions below. If you do see it, click on the tangent icon once. Then right click anywhere in the window, and choose Delete. This will give you a chance to practice adding constraints.
You want to ensure that the curve you just created is tangent to the hypotenuse of your triangle. In the first image, notice that there are two overlapping lines in the yellow box. This would cause modeling problems later.
1) In the Sketch palette on the right, choose Tangent.
2) Click the curve, and then the hypotenuse.
Notice the tangent icon now appears at the intersection of the line and arc.
3) Right click, and choose OK to exit Tangent mode.
Step 14: Trim Area Around Arc
1) Enter hotkey T to activate Trim tool.
2) Select the bottom edge of the hypotenuse that you want to trim.
3) Select the portion of the bottom leg that you want to trim.
Note that a pop-up will appear in the bottom right corner after steps 2 and 3, saying that a constraint was removed. The coincident constraint was indeed removed in this trim operation, but that's fine.
4) Right Click and select OK to deactivate Trim tool.
Step 15: Stop Sketch
1) Inspect your sketch and ensure that the dimensions are correct.
2) In the ribbon, click Stop Sketch to exit the edit Sketch state.
The dimensions will no longer appear on the screen.
Step 16: Extrude
1) In the Create dropdown, choose Extrude.
2) Click the Home icon on the View Cube to see the extrude from an isometric perspective.
3) Click the area of the push stick that you want to extrude.
4) Enter 0.75 into the Distance box to specify the distance of the extrusion.
To extrude in the other direction, you can always enter a negative number for distance. Positive and negative values are determined by the Right Hand Rule.
5) Hit Enter to complete the extrusion and create a solid model.
Step 17: Create New Sketch
Now you will create a pocket feature--an arrow that shows you which direction to use the push stick. This will give you more modeling and CAM practice.
1) Right click the side of the solid model and choose Create Sketch.
2) In the ribbon, choose Sketch>Rectangle>2-Point Rectangle.
Alternatively, use hotkey R.
3) Draw a rectangle to the right of the open circle. This will be the base of the arrow.
As you draw the rectangle, enter dimensions 0.75 for the height and 2.5 for the width. You can dimension objects as you draw them--just like you did when you created the circle. Or, you can roughly draw the rectangle, use hotkey D, and create dimensions after the fact.
Note that vertical and horizontal constraints have automatically been applied to the rectangle: you can tell by matching the icons next to each edge with the constraint icons in the Sketch Palette.
Step 18: Sketch Arrow Part I
1) Use hotkey L to activate the line tool.
2) Off to the side, draw a closed triangle. You will move it into place as the head of the arrow later.
3) Use hotkey D to activate the dimension tool.
4) Dimension the vertical side to 1.75.
5) Click the points on the far right and the bottom of the triangle to create a new dimension.
6) Rather than entering a number here, when the cursor is active in the dimension box, click on the 1.75" dimension you just created. A numbered dimension should appear in the dimension box--in my case, d15. Now, type "/2" after that dimension to divide it in two. Hit enter.
You just created a function. This means that anytime you change d15--the back of the arrow head--the front of the head will proportionately scale. It's a great practice to use functions as much as possible to make your designs more easily editable.
Step 19: Sketch Arrow Part II
1) Drag the triangle near the right side of the rectangle.
2) Use hotkey D to activate the dimension tool.
3) Click the top left corner of the rectangle and the far right vertex of the triangle, then move the cursor right and click to create a dimension.
This dimension should be vertical--the dimension arrows will point up and down.
4) Again, rather than typing a number, click the dimension for the height of the rectangle, 0.75"--for me, d9--and type "/2" to divide it by two. Hit Enter.
The text for the dimension should be "fx: 0.375." This will ensure that the triangle is vertically aligned with the rectangle.
5) Select the Colinear constraint in the Sketch Palette on the left side.
6) Click the right side of the rectangle and the left side of the triangle to make them colinear.
This will ensure that the triangle is horizontally aligned with the rectangle.
7) Right click and choose OK to deactivate the colinear tool.
8) Drag the arrow to the exact location where you want it, ideally evenly spaced between the circle and the right edge of the push stick.
9) Use hotkey T to activate the trim tool.
10) Click twice to remove the lines between the rectangle and triangle.
Don't worry if you delete constraints in this process.
11) In the ribbon, click Stop Sketch to exit the edit Sketch state.
Step 20: Second Extrusion
1) Click the home icon by the view cube for an isometric view.
2) In the ribbon, choose Create>Extrude.
Alternatively, use hotkey E.
3) Click the inside of the arrow, and type -0.25 for the extrusion distance.
Notice in the Extrude window that the Operation has turned into Cut, because you entered a negative value. You can use the extrude tool not only to add material, but also to cut it out, join two objects, or create new models from intersections.
4) Hit Enter to create the extrusion.
The geometry you just created is called a pocket because it is bounded by a contour and has a flat bottom.
Congratulations! You are done modeling the push stick.
Step 21: CAM Workspace Adjustments
1) In the ribbon at the left, change the Workspace to CAM.
CAM (Computer Aided Manufacturing) is the way you will create toolpaths to machine this part on the Shopbot.
2) Orbit or click the view cube corner where Front, Right, and Bottom intersect. This is an isometric view of the part, with Z pointing up.
3) Right click the home icon next to the view cube, and choose Set current view as home>Fixed distance.
You want to view the part as it will appear when it is machined, and as you know from the Right Hand Rule, Z points up. For the Shopbot and other 3-axis CNC machines, this means that the cutting tools will always be normal to the XY plane.
4) In the browser on the left, click the icon next to Units to change the units to inches (again--you have to do this in each Workspace), and click OK.
Step 22: CAM: Setup Part I
There are three steps in the CAM process: Setup, Toolpath, & Simulate.
Setup determines the location of the Work Coordinate System (WCS) and the size of your raw material (stock).
Think of the Work Coordinate System as the way that you locate your stock when you place it on the Shopbot. The bed of the machine is 4' x 8', but your stock might be much smaller. For this reason, you must tell the machine where your part is located by setting a home location, which is the origin point of the Work Coordinate System. This origin, also called the Work Home, is often placed on one of the top corners of the stock.
1) In the ribbon, click Setup (the icon on the far left, above the Setup dropdown).
In the graphics window, the box surrounding the model--which represents the stock--contains many nodes. These nodes are potential locations for the WCS origin (Work Home).
2) In the Setup window, next to Origin, choose Model box point.
3) Click the top front left corner of the part, as shown in the screenshot. Do not click OK in the window.
This moves the WCS origin to the top front left corner and defines its X, Y, and Z coordinates. Note that the x-axis points along the long axis of the part, the y-axis points away, and the z-axis points up, following the Right Hand Rule. This X, Y, and Z orientation is important and you'll need to remember this when you place your stock on the Shopbot. For a more detailed explanation of the Work Coordinate System, watch this video: Setting up a Work Coordinate System.
Step 23: CAM: Setup Part II
You will use the Setup window tabs the same way you read--going from left to right. You've already set your WCS, so now it's time to define stock.
1) Click the Stock tab.
2) Change Mode to Fixed size box. Before selecting it, hover your mouse over it to read the explanations.
In general, if you see a parameter that you don't understand, you can hover your mouse over it to see a definition. Fusion is pretty good about offering explanations for terms, many of which include diagrams, to guide you.
3) For the purpose of this exercise, enter 24 for Width and Depth, and 0.75 for height.
If you plan to actually machine this part, now is a good time to find your stock, which should be a piece of 3/4" plywood that is larger than 15" in both X and Y. The largest dimension of the part is a bit more than 11", but you want to leave room for your fixturing system (the way you will hold the part down to the Shopbot table). Measure your stock and enter these dimensions into the X and Y values. It's fine if the stock is much larger than you need--no need to cut it down. It's important to be in the habit of having accurate stock sizes in CAM.
Otherwise, stick with 24" x 24" x 0.75" for now. Later, when you get your stock, you can easily update the setup with accurate dimensions.
4) Under Width (X), change Model Position to Offset from left side, and change Offset to 1.
5) Under Depth (Y), change Model Position to Offset from front side, and change Offset to 1.
On the Shopbot, after you home the machine, the spindle will be oriented above the front left corner of the machine bed. It's a good habit for you to place your stock in this corner of the Shopbot machine bed.
For the sake of consistency, you just placed your part in the front left corner of the stock. You added an offset of 1" in order to ensure that there is sufficient room for the outer contour of the push stick in the stock material.
6) Click OK to generate Setup.
Step 24: 2D Pocket Part I
The next step after Setup is Toolpath.
1) In the ribbon, choose 2D>2D Pocket.
2D Pocket is a roughing toolpath that creates toolpaths parallel to selected geometry.
The browser that opens, with 2D Pocket at the top, is the way that you will control all the settings for this toolpath. Hover your mouse over the tabs to see their names: Tool, Geometry, Heights, Passes, and Linking. It's a good practice to navigate the tabs from left to right, like reading a book. In your current tab, the Tool tab, you will choose your cutting tool and specify the speeds and feeds for that tool.
2) In the browser, click Select next to Tool.
3) If needed, expand the left side of the window by clicking the "Show Library Tree" icon in the top left corner.
4) Make sure all the Samples libraries are de-selected, except for Inch--Aluminum.
5) Choose the 1/4" flat Endmill from the Samples/Inch--Aluminum library, and click OK.
6) Change Spindle Speed to 12,000 rpm, and Cutting Feedrate to 75 in/min.
Because you are choosing this endmill from a Sample library, you cannot be sure that the default speeds and feeds are correct. For your own projects, refer to the Shopbot feeds and speeds chart to ensure that your spindle speed and feed rate are correct for your particular endmill and material.
Step 25: 2D Pocket Part II
1) Click on the Geometry tab--the next tab next to Tool.
In this tab, you will choose which geometry to machine within the current toolpath.
Refrain from pressing "OK" between tabs, because that will generate the toolpath. If you accidentally do, find the toolpath on the left under Setup 1 in the CAM Feature Tree, right click, and choose Edit to go back to the browser.
2) You are being prompted to make a selection. Carefully click on the bottom contour of the arrow--not the face. It's generally more accurate to choose contours than faces.
The arrow will fill in a dark blue color. This means that this is the area to be machined, which is what you want.
3) Click on the Passes tab.
In this tab, you will control how the tool behaves during each pass.
4) Change Maximum Stepover to 0.125.
For machining wood or plastic, follow the Stepover and Stepdown Rule: The stepover and stepdown should never exceed 50% of the tool diameter.
In this case, the tool diameter is 0.25", so the maximum stepover is 0.125".
5) Check the box next to "Multiple Depths" to activate it.
This means that the tool will not attempt to machine in a single pass, but rather step down multiple times.
6) Change Maximum Roughing Stepdown to the correct amount.
You should know this from the Stepover and Stepdown rule--check screenshot for answer.
7) Uncheck Stock to Leave.
Because Pocket is usually used as a roughing operation, the software will default to leaving a thin "skin" of stock behind that will be removed with the finishing pass. Because you are roughing and finishing with the same operation, you will not leave any stock behind.
Step 26: 2D Pocket Part III
1) Click the Linking tab.
This tab controls the behavior of the tool when it is not cutting.
2) Change the Ramp type to Zig-Zag.
The purpose of Ramps is to slowly descend the cutting tool along the Z-axis, because endmills are much better at cutting radially (laterally) than axially (plunging). Ramps put less stress on tools and give them a longer life.
Helix is the default ramp style and works well in theory. In practice, however, you should avoid Helical ramps when using the Shopbot, because the results are not always consistent.
3) Click OK to generate the toolpath.
A quick guide to the colors of the toolpath:
Blue = The toolpath itself. The tool moves at the cutting feedrate.
Yellow = Positioning moves. The tool moves at rapid or high speed.
Red = Ramp (helix, zigzag, etc).
Green = Lead in/lead out. This is how the tool moves right before or after each cutting move, for a better surface finish.
Step 27: Simulate!
After Setup and Toolpath, the next step is Simulate.
After you create any toolpath, you'll want to simulate it to ensure that it's not colliding, that it moves efficiently, and that it's doing what you expect. Pay attention to where and how the tool enters your material, and how much material the tool is removing at any given time.
1) Click Setup 1 in the CAM Feature Tree.
2) In the ribbon, click Simulate.
3) In the Simulate browser, change Toolpath mode to Tail.
This will remove some of the visual clutter from the screen.
4) Check Stock to make the stock visible.
You can check the box next to Transparent as well--I tend to toggle it on and off, depending on what I'm doing.
5) Press Play.
The slider underneath the Play/Pause controls allows you to speed up and slow down the simulation. Below that is a thin timeline. You can click at any point in the timeline to go to that point. If you hover your mouse over the timeline, it will display the name of the toolpath, the tool number, and estimated machining time.
6) Click Close to exit the simulation.
Step 28: Creating New Sketch for Drilling
Remember that it's impossible to machine sharp inner corners. When you're machining inside corners, you will end up with a fillet whose size is the radius of the tool you're using (see screenshot).
Think about the purpose of the pushstick. You want to be able to firmly and safely push material through the tablesaw. If you have a radius on the inside corner of the "step" of the pushstick, the back edge of your material will not be flush against the pushstick. This would result in an unstable, and therefore less safe, system.
For this reason, you are going to drill a hole in that corner. This is called a dogbone--a style of machining that allows you to remove inner corners for a variety of applications.
Notice that there is not a hole in the solid model itself, so you will need to create a sketch that specifies where your hole will be drilled.
1) In the ribbon, change the Workspace to Model.
2) Orbit to the back side of the pushstick (no arrow), right click on the face, and choose Create Sketch.
3) In the ribbon, choose Sketch>Point.
4) Click the inner corner of the "step."
5) In the ribbon, click Stop Sketch.
Step 29: Drilling
1) In the ribbon, change the Workspace back to CAM.
2) Note the red exclamation point in the CAM Feature tree to the left of 2D Pocket1.
Because you changed something in the Model Workspace, you will need to regenerate the toolpaths you've already created.
3) To do this, right click Setup 1 and choose Generate Toolpath.
4) In the ribbon, click Drilling.
5) In the browser, click Select next to Tool.
6) From the Samples/Inch Aluminum library, choose a 1/2" Drill and click OK.
7) Change the Spindle Speed to 1000 rpm.
By default, drill rpm is not correct. Use the following schedule for Sample Library drills:
1/8" Drill: 4000 rpm
1/4" Drill: 3000 rpm
3/8" Drill: 2000 rpm
1/2" Drill: 1000 rpm
8) Click the Geometry tab.
9) Change Hole Mode to Selected Points.
10) Select the point you just created in the inner corner of the "step".
Step 30: Drilling Part II
When you select a point for your hole geometry, you have more parameters to change in the CAM software than if the hole were already part of the solid model. Specifically, there is more to do in the Heights tabs.
1) Click the Heights tab.
2) Change Top Height to Selection.
This is because "hole top" does not exist--you just have a point.
Note that the Offset will have a red error, saying "invalid reference." This is just prompting you to make the reference, which you will do in the next step.
3) Click the top face of the pushstick.
4) Change Bottom Height to Model Bottom.
Note that the dark blue rectangle representing Bottom Height appears in the window.
5) Check Drill Tip Through Bottom.
A standard drill bit has a 118 degree angle at the end. By default, the drilling toolpath will end exactly at the tip of the drill. In this case, this means the drill would not go all the way through the model. By checking this box, the drill bit will continue past until it's created a complete hole through the model.
In general, you would use a spoiler board (scrap board) under your part on the bed of the CNC machine to prevent machining into the machine bed. However, it is OK to machine (lightly) into the Shopbot machine bed at Pier 9. Never machine into the bed more than 0.05".
6) Add a break-through depth of 0.02.
The break-through depth specifies how much further the tool drills past the bottom of the hole, after it has broken through.
7) Click the Cycle tab.
8) In the dropdown, hover your mouse over any cycle to read about the cycle types.
9) Change the Cycle type to Deep Drilling-Full Retract.
Though new fields will appear, leave those at the default settings.
The default drilling cycle is Drilling-rapid out. This brings the tool into the hole once and then rapid retracts. Deep Drilling, which is more conservative, is the best cycle for the Shopbot, because it periodically retracts the tool out of the hole to allow chips to escape. This will help drill bits last longer.
10) Click OK to generate toolpath.
Step 31: Simulate!
1) Click Setup 1.
2) In the ribbon, click Simulate.
3) Turn off the visibility of the model by clicking the light bulb next to "Shopbot push stick" on the left in the CAM Feature tree.
4) Make the stock transparent so you can watch the deep drilling.
5) Click Play.
6) Click Close to exit simulation.
Step 32: More on Dogbone Joints
Step 33: 2D Contour Part I
Finally, you want to machine the outer contour of the pushstick.
1) Turn on the visibility of the model.
2) In the ribbon, choose 2D>2D Contour.
In type of toolpath, the tool will follow a contour. Contours can be open or closed and can be on different Z-levels, but they must be flat (2D).
3) Click Select next to Tool, and choose a 3/8" flat endmill. Click OK.
4) Change Spindle Speed to 12,000 rpm, and Cutting Feedrate to 75 in/min.
5) Click the Geometry tab.
6) Click the outer and inner contours of the part.
7) Zoom in on the inner circle.
The red arrow represents the direction and side of the contour that will be machined. Right now, you can see that the tool will move clockwise on the outside of the contour. You want the tool on the inside of this contour.
8) To switch the direction and side of the contour the tool will machine, click the red arrow once.
9) From a top view of the part, check tabs.
You want to add tabs to this toolpath to prevent stock from coming loose while being machined. In CNC machining, it's important that your stock and workholding system are always rigid and secure. Loose parts could damage tools or the machine spindle.
You will remove the tabs later with wood shop tools such as a bandsaw, chisels, or jigsaw.
10) Change Tab Height to 0.15.
11) Change Tab Distance to 6.
You only need enough tabs to keep the part in place.
Step 34: 2D Contour Part II
1) Click the Heights tab.
2) Under Bottom Height, add an Offset of -0.05.
You want this toolpath to go slightly below the bottom of the part, and into the machine bed, in order to prevent a thin "skin" of stock material from remaining on the edge of the part. Add this additional offset anytime you machine around the boundary of a part.
3) Click the Passes tab.
4) Check Multiple Depths.
5) Change the Maximum Roughing Stepdown to the correct amount, from what you know of the Stepdown and Stepover rule.
6) Click OK to generate toolpath.
7) Verify, from the side view, that this toolpath does indeed go slightly below the bottom of the part.
Step 35: Simulate!
1) Click Setup 1.
2) In the ribbon, click Simulate.
3) Turn off the visibility of the model.
4) Click >| to skip to the final CNC machined part.
5) Inspect the model.
This is what the part will look like after all machining operations. Zoom into the various parts and make sure they look the way you expect.
Step 36: Post Process Part I
Now that you're sure that your simulation is correct, it's time to post process to convert your CAM file into G-code. G-code is the computer language that CNC machines use to execute a program. Each line is a a different instruction for the machine.
Note: If you're using a Mac, your screenshots will look different. As long as you choose Generic Posts, Shopbot.cps (Shopbot Open SBP), your G-code will be identical.
1) Right click 2D Pocket1.
You will post process each toolpath separately, because you must manually change tools on the Shopbot.
For the Shopbot in general, create a different program for every tool (or every time a tool change is required).
2) Choose Post Process.
3) In the window, click Setup in the top right corner.
4) Select Generic Posts.
5) Under Post Configuration, choose Shopbot.cps--Shopbot Open SBP.
Step 37: Post Process Part II
1) Insert a USB drive into your computer.
2) Click the three dots to the right of Output folder to map the output to another location.
3) Navigate to your USB drive, and click Open.
4) Under program name or number, type 1001--it must be four digits, and only digits.
Because you will have multiple programs, organize them such that Tool 1 goes with program 1001, Tool 2 with 1002, and Tool 3 with 1003. This will keep you organized.
5) Under program comment, write something useful like "Tool 1 pushstick pocket."
6) Click Post.
7) Click Save to save to USB.
Overwrite if necessary--it's not important to save g-code programs. Even if I use the same Fusion file multiple times, I always post just before I'm going to machine.
The G-code will appear in the editor.
8) Repeat these steps to post process the Drilling Toolpath, and save as program 1002.
9) Repeat these steps to post process the Contour Toolpath, and save as program 1003.
Congratulations! You've successfully worked through the CAM for a simple 2D part for the Shopbot. You're ready to start machining, so grab your Shopbot Safety/Basic Use handout and get started!