8. Computer controlled machining¶

Group Work¶

The Group work was done with the whole Oulu 2019 batch. All the picures and measurements related to the group work are taken from Jobin’s and Perttu’s page.

Model.	Machined output.
Outer length measurement.	Inner length measurement.
Inner diameter measurement.	Outer diameter measurement.

Outer Square (mm)		Inner Rectangle (mm)		Outer Circle diameter (mm)	Inner Circle diameter (mm)
L1	L2	L1	L2	Outer Circle diameter (mm)	Inner Circle diameter (mm)
150.11	150.10	120.31	100.14	80.11	59.88
149.92	150	120.08	99.99	80.15	59.92
150.42	150.01	120.05	99.86	80.09	59.85
150.10	150.01	120.13	100.03	79.70	59.76
Average: 150.14	Average: 150.00	Average: 120.14	Average: 100.00	Average: 80.01	Average: 59.85

Individual Assignment¶

This week I designed a box with a lid to store things (how creative). I started with high hopes of making a fully parametric design with dovetail joints. It turned out that making a parametric design does not mean just specifying the needed dimensions as parameters, you also have to make sure that all the sketches are properly constrained with the defined parameters and all the references are from correct place(faces,edges…). I learned this the hard way. Furthermore, the dovetail joints I designed were blind and I didn’t use any T bone or dog bone structures, which meant that I would have to use lot of elbow grease to make the joints fit. And Monday is already gone and now I have to redesign my box with rectangular joints.

Examples¶

For designing, I followed the following videos on youtube and Heidi’s page.

Design Procedure¶

3D design¶

I started the design by defining all the components that will be assembled (bottom, left wall, right wall, etc.). Each component is very simple and just uses a rectangle and an extrude feature.

Defining all the components.

Designing the bottom component.

After creating all the components, I created a box that represents the stock that we will be milling the furniture from. This “stock box” was used to lay all of the parts flat onto. The osb board we are using here is 11m thick, it is 1200mm wide, and it is 2600mm tall. After that, I assigned the stock component to be a “ground” to keep it from moving around. This was done by selecting the stock component from the tree on the left, right clicking, and selecting ground. To lay the parts flat on the stock, I followed the following sequence

I selected assemble –> Joint
I selected the bottom face of the top of the component
I selected the top face of the stock
I picked the top face of the stock
I selected “planar” for the type
and then I pressed “flip” to get the blind pockets facing up.

This was repeated for all the components. To make sure that the components do not lie on top of each other, they were moved too by giving each of them a different X and Y offset.

All the designed parts laying flat.

Dogbones¶

CNC milling tool bits are large in size compared to a laser beam (few mm compared to um). This creates a problem when one wants to cut right angles on an inside edge. The round bit cannot reach inside corners, thus some small amount of material is left. Check this webpage for visuals. To fix this issue, one can make extra cuts in the design so that the round mill bit can go a little bit closer to the edge. When done on a pocket, the resulting pocket looks like a dog bone and thus the name. Keep in mind this is only in design i.e., a rectangular pocket looks like a dog bone to the CNC machine but after machining it will look like a rectangle.

The easiest way to do it in Fusion 360 is by using the Dogbone Plugin. Unfortunately, when I ran that plugin on my design, it crashed. However, it is not very tedious to make them manually, if kept in mind while doing the design. For my next project I will definitely keep this in mind. Below is shown how to draw a dogbone on one side of a pocket

For manually making a dogbone, first create a circle which has the same diameter as the tool. Then create a construction line from the edge of the corner to the center of the circle. Next, create another circle with the same diameter and make the center of it coincident with the construction line created previously. Next, make sure this new circle touches the edge of the corner where one wants to create the dogbone. Next, extrude away the extra parts (the deep blue parts in the second image below). The example file is attached below.

Creating a construction circle having a diameter equal to the tool.

Creating a second circle with the same diameter, using the first one as a guide.

Part after extruding the extra material.

Nesting¶

According to wikipedia

In manufacturing industry, Nesting refers to the process of laying out cutting patterns to minimize the raw material waste.

In my design, I have done the nesting manually where I manually placed all the different parts of my box on the ground stock. However, doing it manually is not the most efficient way and there is a Nesting Plugin for Fusion 360 which can be used for doing the same.

CAM settings¶

For creating the tool paths for milling, I downloaded the CAM processor file and the setting files with values for different milling bits (included below) from the Fab Lab Oulu Wiki site and added them to the Fusion.

Importing the tool library.

Setup¶

In the Fusion’s manufacture workspace, I created a new setup via SETUP>New Setup, where Operation type, Orientation, Origin, and Box point were set under the Setup options. Under Stock options, I changed all the offset values to 0mm. It is important to ensure that the Height (Z/vertical axis) is the width of the actual board that will be milled.

Setting up the stock and origin.

Pocket¶

Under 2D>2D Pockets dialogue box in the Tool tab, choose the milling bit, which is the 6 mm flat bit. Under Geometry tab, select the areas where you want to make tabs/pockets. Under the Clearance Height tab, set the top and bottom heights. In Passes tab, set the maximum depth for drilling using even step downs. Under Linking tab, deselect Leads and Transitions and set the Ramp Type to Plunge.

Creating tool paths for making a pocket.

2D contour¶

To make half depth slots, I used 2D>2D Contours. Most of the settings were similar to those in the 2D pockets, with only difference in the Bottom height under the Clearance tab.

Creating tool paths for making half depth slots.

2D>2D Contours was also used to cut the rest of the parts. Here too the only different setting was the Bottom height under the Clearance tab, which was set to Stock Bottom.

Creating tool paths for making different parts of the box.

Creating tool paths for making the bottom of the box.

Simulation and file generation¶

After making all the tool paths, the tool paths were simulated to check any abnormalities. After that the post processor file was created which is required by the CNC router.

Simulating the tool paths.

Cutting¶

The CNC machine used is RE2-1325 CNC Router With Linear ATC. Below is a picture of the warning labels on the machine.

Warning labels.

First you turn on the computer connected to the CNC machine, then the machine’s power switch and main switch are turned on.

Main power switch.

Powering up the machine.

On the computer, start the NC Studio program, and then reset all the axis so that the machine knows the limit of the xyz axis.

Resetting the axis.

Next, place the material board with screws on the sacrificial surface of the CNC machine.

Firmly securing the work piece.

Next, place the desired milling bit in the CNC tool collet and placing the collet clamping nut followed by tightening them using a spanner.

Tool used.

Endmill attached and the collet clamping nut placed.

This is followed by setting the X and Y axis and calibrating the Z axis. Automatic calibration in the NC studio program was used for the Z axis.

Setting the X origin.	Confirming the new X origin.
Starting Mobile calibrator for the Z axis origin.	Click yes to continue.
Placing the mobile calibration unit under the endmill and automatically setting the Z origin using mobile calibrator.

Load the .nc file on NC Studio program and simulate it.

Loading the nc file and simulating it.

To start cutting, first switch on the vacuum pumps and the dust collector and then press PLAY. Keep the spindle speed to roughly 70% when starting the cutting.

Setting a low spindle speed at start.	Machine making pockets.
Machine cutting.	Machine cutting some more.

When the material is cut, switch off all the units. Use a knife to remove the tabs.

Freeing the boards by cutting the tabs using a knife.

Assembly¶

After some sanding and filing the edges and tabs, I assembled the complete box. Given the fact that I haven’t used any dogbones, some elbow grease was required for sanding and hammering in order to fit the panels which explains the tight fit. Furthermore, given the fact that the material used was an OSB board which chips really easily, finishing was not the best.

Fully assembled box.
Another view. Finishing could have been better.	Another view.

Speeds and Feeds¶

Process	Speed (rpm)	Feed Rate (mm/min)
Pocket	15000 (max)	9000 (max)
2D contour	15000 (max)	9000 (max)
Actual values at the router	10500 - 12000	2500

Problems¶

For some reason, while generating the tool path for the bottom part of the box, instead of one continuous contour, there were multiple contours and I was not able to automatically select all of them via the chain selection, so I had to manually select them. However, while doing so, I managed to skip some of the contours, which made the shown holes on the bottom plate.

Problem edges.

Problem edges at the bottom.