Pier 9 Guide: 2.5D Workflow: Inventor to Shopbot

This Instructable is for Workshop Users at Pier 9.

Requirements for using the CNC machines at Pier 9

• Take General Workshop Safety Class.
• Take relevant CNC Basic Use and Safety Class(es).

This Instructable will teach you basic 2.5D milling techniques in Autodesk Inventor HSM, from setup through post processing for a Shopbot CNC router.

This is a great workflow for beginners to CNC who want to practice CAM programming before embarking on their own designs. Using the Inventor model provided below, CAM_practice_part.ipt, you can follow these step-by-step instructions to prepare your CAM (Computer Aided Manufacturing) file using 2D toolpath techniques, including Facing, Pocket, and Contour.

This Instructable was created at the Pier 9 workshop using Inventor Pro 2016 HSM. If you have access to a CNC machine and Inventor, you can download the plugin Inventor HSM Express for free, which will allow you to use 2D and 2.5D CAM strategies. Let's begin!

1. Download the practice part and open it in Inventor. The default unit is inches. Note that this model is 2.5D, meaning that all our toolpaths will lie flat along the xy-plane. The z axis will only be used to position the tool at depth.

2. Ensure that you're in the CAM tab at the top of the screen. The three main steps in CAM are Setup, Toolpath, and Simulate. To start, this means we're going to click Setup, in the ribbon at the top of the screen.

3. During the Setup phase, we will determine the size of our stock, the location of our part within our stock, and the location of our Work Coordinate System (WCS). The Work Coordinate System allows the programmer to program the part away from the machine, and tells the CNC machine where the part is located within the machining envelope. Even though it's common practice to set your WCS (indicated by the x, y, z triad) on a corner of your stock, for this operation we're going to assume that we're milling into a 1/2" thick piece of sheet material, like MDF, plywood, or corian. Because we don't know where our part will be located in this sheet, and because we might mill multiple times out of the same sheet, we're going to set our WCS in the center of the part. Ensure that Orientation is set to Model orientation and Origin is set to Stock box point.

4. In the Stock tab to the right of the Setup tab, change Mode to Fixed size box, and enter 20" for X, 20" for Y, and 0.5" for Z. For model position, choose "Offset from top (+Z)" and enter an offset of 0.05". This places the model 0.05" below the top of the stock. By positioning the part just a bit below the top of your stock, we can ensure that our part will be flat with consistent dimensions.

5. Click OK to finish Setup. You will see the Setup folder appear in the CAM Feature Tree on the left side of the screen.

1. To face our stock, which is the most common first toolpath operation, click Face in the 2D milling section of the ribbon on the top of the screen.

2. Choose a 1/4" flat end mill as your tool. Because this design is 2.5D, you don't need an endmill with a radius. (If you're at Pier 9, you should download the Pier 9 Tool Library by following the steps in Dan Vidakovich's great Instructable here. Choose an end mill from the DMS Tool Library, not the Haas Tool Library. Though you'll be using the Shopbot, the feeds and speeds should be a good starting point.)

3. While still in the Tool tab, change the plunge feedrate to 20 inches/minute. By default this is set too high, and we won't be using ramp strategies when machining our part so we want a slow, conservative plunge feedrate.

4. In the Geometry tab, choose the three top faces as your Stock Selections. They will be highlighted in yellow. This constrains the toolpath to this area of the stock, so you're not facing the entire 20" x 20 " surface.

5. Click OK to create the toolpath.

6. Now you want to simulate your toolpath to verify that it's correct. Click Setup in the CAM feature tree, and then click Simulate in the ribbon above. Use Toolpath Mode "Tail," activate your stock in Standard Mode, and use Colorization: Operation at first, toggling between transparent and opaque stock. Pan and zoom around the model as you watch the simulation, carefully watching the path of the end mill. Especially pay attention to the places where the tool enters and exits your material, and visualize how your stock is going to be clamped to your spoiler board. If you're using toe clamps, will be they be near the toolpath? If you're using screws to hold your part down, is there a chance that the endmill will collide with them? If you must have screws near your part, you can use brass screws, which are softer and not damaging to CNC tools. If the tool turns red at any point, or you see red marks in the timeline at the bottom of the screen, the software has detected a collision (either between the stock and the tool holder or because the tool is descending below the top of its flutes, where it can no longer cut). In this case, you will need to exit the Simulation and right click on your toolpath to edit it. You may need a longer tool.

1. Click 2D Pocket in the top ribbon.

2. Use the same tool as you used in the Facing operation, which is selected by default.

3. While still in the Tool tab, change your Plunge feedrate to 20 in/min

4. Referencing the image above, carefully select the three pockets which are the "shoulders" of the design. Make sure you're selecting the entire plane of the pocket, which has an inner and outer contour.

5. In the Passes tab, change Maximum Stepover to 0.125", which is 50% of the diameter of the tool we're using. Also uncheck "Stock to Leave," which ensures that this toolpath will not leave any stock behind. This toolpath is going to serve as both a roughing and finishing pass.

6. Click OK to create the toolpath.

7. Click Setup in the CAM feature tree, and then click Simulate in the ribbon above. Play the simulation.

1. Click 2D Pocket in the top ribbon.

2. Use the same tool as you used in the previous operation, which is selected by default.

3. While still in the Tool tab, change your Plunge feedrate to 20 in/min.

4. Referencing the image above, carefully select the face of the two mid-level pockets and the two lowest pockets.

5. In the Passes tab, change Maximum stepover to 0.125", which is 50% of the diameter of the tool we're using. Then, check "Multiple Depths." These pockets are deep enough that we want to step down multiple times within our toolpaths. Change Maximum roughing stepdown to 0.125" as well. Finally, uncheck "Stock to Leave".

6. In the Linking tab, change Safe Distance to 0.001". This ensures that the lead-ins and lead-outs do not interfere with the part. (By default, these links actually would carve into your part. As an experiment, see what happens when you leave this number at the default. Simulate, and check Part comparison to see where the gouges are--they show up in red).

7. Click OK to create the toolpath.

8. Click Setup in the CAM feature tree, and then click Simulate in the ribbon above. Play the simulation to verify your toolpaths.

1. Click 2D Contour in the top ribbon.

2. Use the same tool as you used in the previous operation, which is selected by default.

3. While still in the Tool tab, change your Plunge feedrate to 20 in/min.

4. Select the geometry of the contour. Then, click the "Tabs" box to create tabs to hold the part in position during this final contour. Otherwise, the part would get loose in the stock while the end mill is still moving--the part could go flying, get jammed or damaged, or it could damage the end mill. For shape, choose triangular tabs, 0.25" wide and 0.1" tall, positioned at a 2" distance.

5. In the Heights tab, under Bottom Height, choose a Bottom offset of -0.05". This will ensure that the endmill goes all the way through the part and slightly into the spoiler board below, preventing a thin "skin" or flashing from appearing at the bottom edge of the part.

6. In the Passes tab, click "Multiple Depths" and choose a Maximum roughing stepdown of 0.125".

7. Click OK to create toolpath.

8. Click Setup in the CAM feature tree, and then click Simulate in the ribbon above. Play the simulation to verify your toolpaths. Now that the toolpathing is finished, click "Show Part comparison" to see if anything else needs to be machined. Any remaining stock turns blue.

The final step is to post process, which will convert the toolpaths in your Setup into an alphanumeric program in a computer language called G-code. These are the instructions your Shopbot will use to machine your part.

1. Right click Setup, and choose Post process.

2. Click Setup in the top right of the new popup box, and choose "Generic."

3. In Post Configuration, choose shopbot.cps (Shopbot Open SBP).

4. Choose any output folder you want. This could be a folder on your desktop, or a USB to bring your program right to the machine.

5. Choose a four-digit number for your program name.

6. Write a specific Program comment, which could include the date. This will appear in the G-code under the program name, helping you verify which program you're using.

7. Click Post. The program will appear in the Inventor editor, and it will be saved in your output folder.

Your program will save as a .sbp file, such as 1001.sbp.

9. Now you're ready to bring your program to the Shopbot! Remember that once you start operating the Shopbot, you should perform a dry run in the air to verify your program before you start to cut your part. For your reference, a comprehensive guide to learning CNC is Dan Vidakovich's great Instructable: Learn CNC the Hard Way

Have fun!