Step 1 — Set up your model in the Manufacturing workspace
Open the model in Fusion360. In this Guide, we’ll be working with “Miller’s Cube”.
If in the Model workspace, change to Manufacture by clicking on the “Model” dropdown in the top left corner of your screen.
To begin your setup, select the “Setup” dropdown in the upper left hand corner, and click on
Step 2 — Setup your Stockbox
Click on the “stock” parameter to set up your stockbox to match your actual stock size.
Select the dropdown menu next to “Mode” and choose the mode that works best for your project. For the cube, we will be working in “Fixed size box” mode.
Enter the width, depth, and height of your stock. The cube has measurements of 1.5″ in all directions.
Adjust the “Model Position” for each axis to match where you would like your model to be placed within your stock box.
For the cube, the X and Y model positions will be “Center”. The Z model position should be “Offset from Top” by .05″
Step 3 — Specify your datum point
Select the orientation of the Work Coordinate System (WCS) for your first setup. For the cube, we will be using the model orientation.
The direction of the axes in your setup orientation need to match the direction of the mill axes of motion.
Select your datum point. You can change your mode of selection by choosing the dropdown next to “Origin”. For the first setup of the cube, we will be using the center of the stock box point as our origin.
Select your model by clicking on the box that says “Nothing” next to “Model”, then clicking on your model. Ensure that all of the parts of your model are selected.
Step 4 — Set up your Post Processing plan
Click on the “Post Process” parameter.
The Program Name/Number must be a number–traditionally 5 digits.
A good practice is to have parts that have multiple setups have related numbers. For example, the cube has 3 operations. They could be numbered 11111, 11112, and 11113 to show that they are related to each other.
The “Program Comment” is what will show up as the name of the program. This should be descriptive of the part and which operation this setup is. The cube can be “Miller’s Cube Op1”.
Step 5 — Begin your toolpaths with a Facing pass
The first step to most first operations is to take a facing pass to flatten and smooth out the face of your stock.
Click the “2D” dropdown menu and select the “Face” toolpath.
The first step to creating any toolpath is selecting your tool. We will be building all of the tools for our program from scratch.
To open the tool library, click on the “Select” button next to the “Tool” option.
Step 6 — Build your tool library
We will build a tool library that is specific to the tools we will be using for this part. Some shops have tool libraries that you can download.
In the right hand corner, there is a series of symbols with plus signs. Click on the left-most symbol.
First we will add a 1/2″ flat end mill. This will be Tool number 1 under the “Post Processor” tab. Tab over to “General” and name your tool 1/2″ FEM
Tab over to “Cutter”. Change the tool type to “flat end mill”.
The parameters of the geometry of your tool should generally match the parameters of your physical tool. We are most concerned with diameter and flute length being accurate.
All of the rest of the defaults can remain unless Fusion forces you to change another value.
Tab over to “Feed & Speed”
Adjust your surface speed and feed per tooth to match the appropriate material, based on manufacturer’s specifications. You may need to adjust your spindle speed down to the maximum capacity of your machine, if you have exceeded it.
Ensure that your ramp and plunge feedrates are roughly 1/3 of your cutting feedrate.
Step 7 — Build the rest of your tools
Click “OK” to complete the build of your first tool. Then click on the “New Mill Tool” button again.
The other tool used in the Miller’s Cube is an 1/8″ flat endmill.
Repeat Step 6 for the 1/8″ endmill.
Under “Post Processor,” this should be tool 2.
Don’t forget to adjust your diameter and flute length, and your feeds and speeds! Click OK when done.
Click OK one more time to complete your tool table.
Step 8 — Geometry Parameter
Click the second symbol in your facing toolpath to adjust your geometry parameters.
When setting up a facing pass, do not select any geometry! Fusion (and most CAM software) will automatically face your stock down to your model.
If you do select the top of your model as your geometry, the toolpath will likely miss facing some of your stock.
Step 9 — Heights parameter
Select the third symbol in the facing toolpath–the heights parameter tab.
You do not need to change any heights for this step, but we’ll go through what they are. In Fusion, you can also hover over the options for descriptions.
Clearance height: the first height the tool rapids to when it begins its toolpath. This is generally well above your part
Retract height: where the tool retracts to before the next cutting pass.
Feed height: where your tool changes from Rapid mode to Feed mode before your first cut.
What is “Rapid mode”?? Rapid mode is when a CNC machine is moving as fast as it can in all of its axes at once. Fed motion is when you have an established feed rate. In manufacturing, you want to rapid as much as possible to save time whenever you’re not cutting.
Top height: the top of your cut.
Bottom height: the lowest your cutter may go.
Step 10 — Passes Parameter
Click on the next parameter tab, “passes”.
Reduce your stepover to 50% of your tool diameter.
Stepover of your tool is how far the tool “steps over” as it moves around your part. Ideal stepover is determined by the type of path you are taking and the type of tool you are using.
50% of your tool diameter is a good stepover for a flat endmill. 75-80% is ideal for a tool like a face mill, whereas a significantly smaller stepover is ideal for a 3D contoured pass, like a scallop, with a ball endmill.
Move onto the final parameter, “Linking”
Step 11 — Linking Parameters
Linking parameters are where we adjust how individual parts of a toolpath are connected to each other.
Important parts of linking parameters include “Keep tool down” and “lead-in / lead-out”
“Keep tool down” indicates that you will keep the tool down at your part through the entire toolpath. In this case, it means that the tool will not retract each time it changes direction. Ensure the box is checked.
The lead-in and lead-out are how your tool approaches and leaves its cutting path. We are not going to change the lead-in or lead-out for this toolpath.