4. Computer Controlled Machining#

This week I participated in a Computer Numerical Control machine (CNC) workshop, in which the goal was to learn how to operate the machine safely and create my own design and cut it.

Tutorial#

Fusion 360#

In order to use the machine we installed Fusion 360 from the AutoDesk website. A student email gives you a year’s free use of the software. First, we used a pre-made shape to learn how to define the cutting path of the CNC.

Setup#

Inside of the “Setup” functionality, we can define the axes of the base that we will be using. We have to define the x axis to go along the longest side of the object and the z axis along the short side. This is because the machine has a very limited space along the z axis, but its longest side is the x axis, so it will have space to move. To do this, click on the first icon above the setup, as seen below. Then, under Work Coordinate System, select X and Z axis then click on the side of the design to define the axes.

This is the base before modification.

This is the base after modification.

Defining the stock#

As seen in the last picture in the “Setup” section, we can also define the stock, under the “Stock” section of the setup tab. The goal is to put accurate measurements of the stock that you have. This allows us to define everything properly in the software, without worrying about hitting the screws that will hold the wood piece in place.

Defining the tool#

When you define a cut path for the machine, you will also have to add the tool it has to use. This allows you to adapt the path to the tool, so that you do not break the tool. The specifications of the tool are given by the manufacturer. In our case, these were the specifications:

Then, you have to define the speeds at which the tool works. In our case, it would be cutting wood. So, we use the speeds that the instructor knew worked from experience:

It is also important to note that, to maintain the tool, you should only go to 3mm depths. We will see later how to control this.

We now have selected the tool and the speed at which we will use it, as seen below:

Face#

In this section, we will define the two faces of the block. This is done in the 2D tab, under “Faces”. The first thing to do is to define the tool used. Then, in the third tab, in “Stock Contours”, select the contours of the bottom and top faces of the object. This will cut the stock to the height it needs to be.

Then, we define the maximum depth the tool should go to. As defined above, this is 3mm for a 6mm tool. This is done in the “Multiple Depths” section of the “Passes” tab:

Pockets#

To define the holes that need to be cut out, we use 2D Pockets. Under the “Geometry tab,” you select the pockets you want to cut out:

Then, you need to define the top height from which the pockets will need to be cut. For this we select the top face of the shape, under the “Top Height” section:

And you need to uncheck the “Stock to Leave” option that leaves a small amount of stock on all the cuts that it makes:

However, we can see that the pocket function left a side of a hole uncut. This is because the width of the hole is smaller than the diameter of the tool. We need to change tools to a smaller one in order to cut this side:

We repeat the same steps, this time with a 3mm tool. For this 3mm tool, the maximum depth the tool can reach is 1mm, in order to preserve its shape. We also need to check the “Rest Machining” option for it to remove only the parts that we have not removed before.

Finally, the last two pockets to define are the two holes on the open hole on the top of the piece. This is done in the same way as before.

In the end, the piece will still have rounded edges cut, since there is no way to make a perfect right angle with a rounded piece.

2D Adaptative#

The last pocket we need to cut out, has no 4th wall. This makes the 2D Pocket function slow and unpractical. Instead, we use the 2D adaptative function. We select the contour of the designed shape and the open chain that defines this hole.

2D Contour#

To cut out the outside of the piece, we use a 2D Contour, selecting the bottom contour of the piece as a closed chain:

By default, the contour is done in layers. However, since we want to prevent the drilling vertically, we can instead ramp down progressively. This is defined in the “Linking” tab. Disabling entry and exit, we can then enable the ramp functionality with the following parameters. Importantly, the Maximum Ramp Stepdown is 3mm, since the 6mm piece we use can only go into the wood until a 3mm depth for the preservation of its structure, as previously explained.

This is the end result:

Finally, we add tabs to hold the piece in place while cutting:

Preparing the files to send to the CNC#

The file to use for the CNC is generated until the “Post Process” functionality. In this, we choose the post we will use which is the “Kinetic NC” one. Then, we choose a location to save the file in.

This file is an NC code which specific instructions in each line that tell the machine where to go and what to do. For example, we can check that the maximum and minimum height are not absurd in order to ensure the correct usage of the machine.s

My piece#

Sketch#

I designed my own piece meant to be a case for my rings. I measured the diameters of my rings so that the holes could be big enough to encase the biggest ones. At first, I wanted to use OpenSCAD to design my piece, since I was already familiar with the design tools. However, when I wanted to transition from a “.stl” file to a file that Fusion 360 could read, I encoutered the problem that the shape was not smooth.

I decided to search how to do this on online programming forums and other social medias dedicated to solving this sort of problem. After some time researching how to open this design correctly on Fusion 360, I gave up and decided it would probably be easier to just learn how to use the Fusion 360 design tool. It is really not that hard to make simple shapes.

Using Fusion 360 I drew the design in 2D, then extruded each part of the design to its corresponding height.

First, I created a Sketch and chose a face to draw my 2D design on.

Then, I drew a rectangle of with the dimensions 90mm and 210mm.

Then, in a different sketch, I drew circles for each ring with diameter 30mm.

Then, I extruded the circles and the background to different heights.

Finally, I rounded the corners.

Toolpath#

Using the methods learnt in the tutorial, I decided to use 2D Pockets and a 2D Contour to define the CNC instructions. The final result is the following.

Then, I produced the NC Code.

CNC#

Having the NC code, I opened it on the computer next to the CNC on the Kinetic NC application.

Next, there is a list of steps to complete in order to properly prepare the CNC for usage:

• Approximate the center of the raw material used and mark it with a cross.
• Place the raw material on the base of the CNC, parallel to the front of the machine. (To do this, use the preexisting lines already etched onto the wooden base inside the CNC.)

• Attach the material to the base of the CNC at 4 points using screws that are long enough to penetrate the whole material, but not too long so as to only drill into the base which is a bit less than 18mm and not the metal casing of the machine. (In my case, since I used a 18mm plank, I used 25mm screws.)

• Load the file onto the computer into the Kinetic NC software.
• Use the arrows of the number pad of the keyboard to align the drill of the machine with the center of the raw material and put the X and Y values of the position of the drill to 0.

• Use the metal button to calibrate the z axis by placing the button centered on top of the raw material and using the first code on the Custom tab of the Application “Z0-finder…”. (If the raw material is too tall there might be a need to place it next to it instead of on top. In this case, the axes should be similarly placed on Fusion 360.)

• Turn on the aspiration machine.

• Press play.

The speed is set manually on the Application, and we were told to use 20000 rpm as explained in the Tutorial above. This worked well. Only on the contour, it was going a bit slowly, so we increased the speed manually. If the speed is too fast or too slow, we risk burning the wood. It results in marks like these found on the base of the CNC:

This is my final piece!