CAM Basics - Machine a Dice!

By Rogelio Castillo Jr.

I am a Junior at Morro Bay High School in Morro Bay, California. Ever since I started learning how to use the CNC Router and CNC Mill at my high school from my sophomore year, I have been more interested in how to use them and have learned plenty. We have a Haas VF2 that many students use often to machine parts and is part of the Engineering classes. So far I have made a few versions of dice, multiple molds for an injection molding machine, and also a set of soft jaws.

The beginner project for the CNC Mill was to make .nc programs for a simple dice. This will be a tutorial primarily focusing on the CAD/CAM portion. The intended purpose is for you to learn the basics of how to use CAM and even CAD depending if you want to design the dice or not.

Note:

Basic knowledge of how to use Fusion 360 will make the steps be more understandable and straightforward.

Googling stuff is highly recommended if you are stuck on a step or want a better understanding of something.

A lot of the variables (Such as how big the dice is, material, tools) can be easily changed. Once you have the understanding of how to make a dice I recommend making your own design. For example, I engraved text on one of the sides.

This instructable will not teach how to operate a CNC Mill. If you are in an engineering class with a teacher and a CNC Mill, I would learn how to use your mill from them. The Titans of CNC Academy and NYC CNC are also great resources to learn everything CNC. Autodesk (Fusion 360) and Haas (American CNC Manufacturer) also have incredible videos.

I recommend to also peek around the menus that may show up so you may have a better understanding of CAD/CAM. Most things in Fusion 360 will have a brief explanation of what they do.

I would recommend to go to this instructible on a separate device (ex. tablet, phone) and go to Fusion 360 on a laptop. There are a ton of pictures and instructions, so be prepared.

Disclaimer:

Remember that CNC Machines can very easily injure/kill you if you are not careful. I am not responsible to any injuries that may occur.

Remember this is also how I have machined a dice and there are many things that are probably sub-optimal and could be improved. I am no professional at all. Take my instructable with "a grain of salt", as people say.

Supplies

Machine & Tools:

I will be using a Haas VF2, although any CNC Mill will work great. A CNC Router theoretically can work too, although it may be more difficult.

A vice (and parallels if necessary) to secure your material/stock. I used the Chick OneLOK.

As for tools, I use a 1/2" Flat End Mill and a 1/4" Chamfer Mill. A 1/8" drill is also used to create the holes in a dice (Because the depth is small I don't use a center drill). A probe is also very useful to set the WCS and tool offsets, and this can be done either manually or automatically.

Material & Program:

Any metal will work adequately. I use 3/4" x 3/4" 6061 Aluminum Square Bar. It is an easy and common metal to machine with and is highly versatile (and arguably a forgiving metal). Here is an example.

Fusion 360. I will use the Design and Manufacture workspaces. Other CAD/CAM programs can also work.

Step 1: CAD (Computer-aided Design) - Design Your Dice

Note: If you want the dice without doing CAD, there is an .f3d model linked below this step.

Create a sketch, then make a rectangle (hotkey is r), then use the dimension (d) feature to make one 0.7". Use the "equal" constraint on a perpendicular side to make it into a square. (Image 1)

Extrude (e) 0.7" to make a cube. (Image 2)

Make the holes on each side of this cube.

a. Side 1 - In a new sketch, make construction lines (L) from each corner, then make a circle at the center with a 1/8" dimension. (Image 3)

b. Side 6- Go to the opposite side of #1 and create a new sketch. This time make 4 construction lines from the corner that connect, then put equal constraints until all lines are equal in length (Image 4&5). From the midpoints of these lines will go two more lines. Lastly, create circles (c) at all midpoints except the very center with equal constraints on all circles, then dimension to 1/8" (Image 6)

c. Sides 2&5, 3&4 - Repeat the previous step for all sides using the same principle (Images 7-10).

4 . Chamfer all edges to 30 thou, or 0.03" (Image 11). This will make the dice look better and act like a deburring step.

5 . Save your design! Name it something cool, boring, or practical!

Congrats! You have created your dice.

Step 2: CAM (Computer-aided Manufacturing) - Setup for Side One

There are a lot of steps here to make an nc program. It will probably be confusing at first, but it gets easier by time. Think of CAM as programming what your CNC cuts. CNC's can generally be called "dumb" because they will do exactly what you program, even if that means crashing the tool directly into the vice (Note: Don't crash anything into the vice).

1. Go into the Manufacture Workspace (CAM) at the top left (Image 1)

2. Create a new setup (Image 2) named "Side One".

a. Machine- In the top of the setup menu, search and select your respective CNC Mill (ex. Haas VF2)

Note: You may need to import a 3d model of your CNC or find it in the Fusion library in the sub-menu.

b. Setup- The Operation Type should already be set to "Milling".

c. Work Coordinate System (WCS) - The WCS can be thought of as the origin of your workpiece and the CNC Mill where all operations will be based off of. By setting the WCS correctly, the piece will be properly machined.

a. Set the orientation to "Select X & Y axes"

b. Select the X axis on a chamfer edge (Image 3) and the Y axis perpendicular to X axis (Image 4). Flip the X and Y axes as necessary to make the arrows of the WCS face into the dice (Image 5). The direction the arrows face is positive coordinates of their respective axis.

c. Make sure the origin is set to be "Stock Box Point"

d. Select the stock point to be at the bottom corner (Image 5).

Model -This is if your model has multiple bodies/components. For our purposes it is unnecessary.

Fixture -This is for when you want to put in a 3d model of your vice. For our purposes it is also unnecessary.

2 . Select the "Stock" tab at the top of the menu. This is what your actual stock would be when actually machining a part. Modify the parameters as necessary for your stock. I used 3/4" x 3x4" 6061 Aluminum Square.

a. Mode- Make the stock "Fixed size box" on the sub-menu.

b. Make the Width (X) and Depth (Y) be 0.7" with the Model Position be in the "Center" for both.

c. Make the Height (Z) 1.1". The Model Position should be set to "Offset from the bottom (-Z)". Set the value to 0.21".

Important Note: The Z offset depends on the length of the top of your vice to the top of your parallels (ex. Image 6), and by giving enough room, the tool will not cut the vice. DO NOT CRASH YOUR TOOL INTO YOUR VICE.

The setup should look like Image 7.

3 . Go to the "Post Process" tab at the top of the menu.

• a. Label the "Program Name/Number" whatever you'd like for organization, but I will make the value "1011".

• b. Change the "WCS" value to 55. This is because G54 is typically set as the origin of the vice, and is never* messed with.

• c. The setup should look like Image 8.

4 . Click "OK" at the very bottom if you haven't already. This will create the setup. Make sure to disable the visibility of your CNC Mill, as I find it gets in the way.

6 . Save your design again! You are ready for making the operations.

Step 3: CAM - Operations for Side 1

This step is to make the first nc program for Side One.

• At the top select the "Face" operation and select your tool (ex. 1/2" Flat Endmill). Facing is self explanatory, as it machines the stock until whatever face you selected on your model.

Note: I downloaded a toolset from "TITANS OF CNC", linked here. Autodesk has a good article on how to import the tool library here. You may need to change the tool number to correlate to your CNC Mill in the real world

Note2: Speeds and Feeds vary drastically from material, tool, and machines. Haas created a great chart regarding this, and even has a video on feeds & speeds, both in imperial and metric. Leave it at default feeds and speeds.

• a. Go to the "Geometry" tab at the top of the menu, then select the face of the top side (ie. Side One, Image 1).

• b. Keep the heights as default in the "Heights" tab.

• c. Go to the "Passes" tab. Make the "Stock Offset" value be 0.2". Scroll to the bottom and select "Multiple Depths" then make the "Maximum Stepdown" value be 0.1" (Applies to 1/2" endmill. This height can probably be increased without breaking the tool). It should look like Image 2.

• d. You can skip the "Linking" tab.

• e. Press OK, and what you will see is the tool path (In blue), and as it says this is the path the tool will cut the material.

2 . Next, select the "2D Contour" operation at the top, which will machine along a contour, as the title states.

• a. Use the same tool with default feeds & speeds.

• b. Go to the "Geometry" tab, and select the chamfered edge as shown in Image 3.

• c. Go to the "Passes" tab, then scroll down to "Smoothing" and select the box (Image 4).

• d. Press OK.

Note: By selecting that specific node, you will cut the sides of the dice to size and also create the chamfers. Digitally it may seems that the chamfered edge will not be perfect, but I have found that making the operation cut exactly along the chamfer will cause burrs. It is not noticeable to leave this edge be rolled. If you have no idea what this means, don't worry about it.

3 . Next, go to the top and select the "2D" submenu, then "2D Chamfer" (Image 5).

• a. Change your tool to a chamfer end mill.

• b. Go to the "Geometry" tab, then select edge shown in Image 6

• c. Go to the "Passes" tab, and enable "Smoothing" just like step 2c above.

• d. Press OK.

4 . Finally, go to the top and select the "Drill" operation (Image 7).

• a. Select your drill.

• b. Go to the "Geometry" tab, then select the hole (Image 8).

• c. Press OK.

5 . Double check your operations make sense by simulating how the tools will actually cut. Right click your setup on the left, then left click "Simulation" (Image 9). If it looks correct, you are doing it right.

6 . Save your design yet again!

Step 4: CAM - Setup for Side Six

This will now be the second nc program. In the real world this means flipping your stock and machining the other side.

• Create a new setup (Step 2.2) and name it "Side Six".

• a. Follow the same steps to create your WCS (Step 2.2c) except the origin.

• b. When selecting the origin type, select "Model Box Point" (Image 1). Your origin does not need to look exactly like mine, but the 6-Side needs to be on top and the arrows of the WCS are going into the dice.

• c. Go to "Stock" tab. The "mode" should already be selected as "From preceding setup". Then, select "Continue Rest Machining", which will use the cut stock from the preceding setup (Image 2).

• d. Go to "Post Process" tab and change the "Program Name/Number" value from "1001" to "1021".

• e. Change the "WCS" value from "54" to "55". This will use G55.

• f. Press OK.

2 . Save the file again, because why not?

Step 5: CAM - Operations for Side Six

This will have the steps for making the operations of the nc program for Side Six. It will be similar to making the operations for Side One.

1. Make a face operation (Step 3.1), making sure you have your 1/2" flat endmill selected. For the "Geometry" tab select the face of Side Six. For the "Passes" tab the "Stock offset" value is set as 0.2" and "Multiple Depths" selected with a 0.1" maximum stepdown. Go back to your previous setup if you are confused (or look at Image 1)

2. (Optional) You can make a separate 2D Contour operation to remove the small lip that is left. This will be detached from the stock (more like a dice now) with the 2D Chamfer operation right below.

3. Make a 2D Chamfer operation under the 2D submenu at the top, then make sure the correct tool is selected, then select the proper geometry like Step 3.3. Remember to enable "smoothing" in the "Passes" tab.

4. Lastly, make a Drill operation, select your tool, then select all the 6 holes.

5. Do a simulation by right clicking the setup and clicking "Simulation", just like last time. If it looks correct, good job! Mine looks like Image 2.

6. Guess what? Save again!

Step 6: CAM - Setup & Operations for the Rest of the Sides

In a nutshell, you have finished the heavy lifting. Because all of the sides are to size and the chamfer is finished for all edges, all you need to do in these operations is create drilling operations for the holes. It is as easy as that. Just follow the previous two steps (except your only operation is the drilling!) for each side, creating new setups, WCS, and Origin each time. If you think you can do it on your own, go for it! The light is at the end of the tunnel (hopefully). Just make sure to save.

It will look something like the image above with all of the operations being visible. Doesn't need to be exactly like it; as long as your operations make sense by simulating them. Great work!

Step 7: Make Your .nC Programs

Now it is time to make your nc programs! These are essentially code that the CNC Mill will follow for actions such as moving from point A to B at velocity X with Tool 987654321 running at Y RPM. You get it.

1. Right click the first setup (Side One) and then click "Create NC Program".

• a. In the pop-up menu, change the "File Name" value to anything you want, or leave it.

• b. Take note on where your NC Program will end up in your system. Default is C:\Users\YOUR_USER_NAME\Documents\Fusion 360\NC Programs".

• c. Click "Post" at the bottom. If your setup and nc program is good, it will let you create an NC Program (Image 2).

Step 8: Double Check Everything

This is technically optional, but I strongly advise to make sure everything makes sense. CNCs are very expensive and you do not want to break one. "There is never a thing as too sure" - Someone, probably.

The areas I can think to look for are:

• WCS

• Origin

• Using G55 instead of G54

• Continuing "rest machining" for your stock

• Operations make sense

• Tools are correct for each operation

• Tool NUMBERS are correct, correlating in Fusion and your CNC.

• etc.

Step 9: Finally Run Your NC Programs

This is where I will unfortunately need to let you go. Like I said at the start, if there is someone to teach you how to operate the CNC Mill, great! There are countless numbers of videos on how to operate any CNC, I am sure of it.

Each NC Program will have to be run separately. This means that you will have to flip your stock accordingly to be correct for the next nc program. Another thing is that you will need to manually set up the WCS (at least for your first op) at the corner of your vice. Put your stock at the same spot as it is in Fusion 360, and you will have a working NC Program. Congrats!

Above is an image of my dice that I made. It has an engraving of "MBHS XC" being an acronym for Morro Bay High School Cross Country. It was a gift to some of the seniors on the team. I hope yours is similarly done and is good.

If you learned something from this, even if it was the CAD design for the dice, good on you! This stuff took me way too long to learn but it made sense eventually (and maybe also a few broken endmills).