In this article, we’ll give you a quick overview of the main CNC milling operations Fusion360 offers, with the goal to help you identify the best ones for your next project.
Please note that there are many valid ways of milling, and that Fusion360 offers other milling operations than the ones we’ll present in this article. We decided to focus on the ones our Mekanika community uses the most on their own CNC milling machines. After reading this article, we strongly recommend that you try different options and see what works best for you.
Preliminary trick: by placing your mouse on the icon of an operation, Fusion360 opens a little help widget with a brief explanation of said operation.
Choosing the right operations for a specific task can be overwhelming given the number of options available. Let’s start with a quick comparison of the basics.
Contour is used to make 2D cuts to free a piece from its stock or to make slots inside the piece. It can also be used to clean the inner edges after an Adaptive Clearing or Pocket operation. Think of it as a release cut you would do with a jig saw.
Pocket 2D/3D vs Adaptive Clearing 2D/3D
Pocket vs Adaptive Clearing
When it comes to milling pockets (basically large holes), you have 2 options: the Pocket operation or the Adaptive Clearing operation.
The main difference between both operations is that Pocket will keep a constant engagement of your mill in the stock, while Adaptive Clearing will take bites, alternating cutting and cooling.
Where Pocket cut constantly (and thus go faster than Adaptive Clearing), the extra time your mill gets to cool down with the Adaptive Clearing allows it to handle bigger steps. The bigger the pocket you are willing to mill, the more time you will save by using Adaptive Clearing instead of Pocket.
This is especially true for hard materials like aluminium or hard plastics.
We recommend always using Adaptive Clearing over Pocket.
2D vs 3D
Choosing between 2D or 3D operation is pretty straightforward: is the volume you want to mill a straight extruded shape, or is there any variance in the extrusion (chamfers, filets, bumps, gaps, slots, etc…)?
If what you want to mill is straight (in top view), then pick a 2D operation. Otherwise, use a 3D operation.
If you use a 2D operation instead of 3D on the conic hole for example, you’ll end up with a cylinder.
Bore vs Drill
The Drill operation will use fixed XY coordinates and plunge in Z. This means that you can only drill out a hole that is the exact same diameter as the end mill you are using, and that dust extraction is not very good.
The Bore operation with plunge in Z while making a helix in XY. This means that you can “drill out” holes that are up to twice the diameter of your end mill. It is also much faster than using a pocket operation for these holes, and will help chips extract from the hole you are drilling out.
To engrave text, logo’s or any other 2D profile in your material, Fusion360 has an Engrave operation. You can learn more about how to use it in our Branding your project.
Milling flat surfaces is a one of the that huge asset a CNC milling machine can offer. Whether you want to use your CNC as a jointer, mill some engineering projects or just flatten your spoilerboard, the Face operation is the one you want to go for.
A CNC machine is not only used for 2D operations like cutting contours or making straight holes, it gives you the opportunity to mill 3D textured projects that would have been impossible to achieve by hand (see our
These kinds of projects are often using a 3D Adaptive Clearing operation first (to rough out the stock), and a Scallop operation with a ball end mill next to refine the texture.
The Scallop operation will make a 3D toolpath around a point and make the end mill travel all around the texture you are willing to mill to get rid of the rice field effect left by a 3D Adaptive Clearing operation.
Though you can use a flat end mill with a Scallop operation, it will leave sharper edges than a ball nose end mill and might leave unwanted cutting marks on your piece that will be very hard to sand away.
Next, let's see how to configure properly those operations
Please keep in mind that these are guidelines. There are an infinite number of possibilities on how to configure milling operations and you will eventually have to tweak these parameters to fit your needs.
As for any operations, you have to start by selecting the end mill you are willing to use for this operation. In our example, we are going to choose an 8 mm flat end mill (from our End mill bundle) for which we will use the hard wood preset.
In the second tab, select the contour you want to mill. If this is an exterior contour, we have to use tabs so that, once the mill reaches the bottom of our piece, the whole body doesn’t come loose (which might be very dangerous).
Change the tabs width, height and spacing until you feel the piece will be sufficiently supported but it won’t be a nightmare to clean after the milling is done. Usually, Tabs every 40-80 mm are enough.
The third menu tab is used to define planes above the model for the end mill to travel when it is not cutting. Editing this tab is optional, but you will eventually have to change these values when using long end mills or when milling really thick stock.
If you are using clamps to secure your stock to the spoilerboard, we advise you not to change these values. If you’ve secured your stock using screws, you can change the value up to the ones shown in the figure below (not less).
In the fourth tab, you should only edit the Multiple passes - Maximum Roughing stepdown value and the Stock to Leave values.
Maximum Roughing Stepdown : we recommend staying under the radius of the end mill you are using (in this case, under 4 mm). As this project would be in hardwood, we will stay safe and take 2.5 mm as step value.
The Stock to Leave is the offset you want to leave between the model and the face the mill is going to cut. This is of course optional.
The last tab is to tell Fusion360 how you want your end mill to enter and exit the stock. In general, we recommend using Ramps instead of Leads & Transitions.
Your menu tab should thus look like this.
If you’ve changed the height values in step 3, you will have to edit the “Safe Distance” value. Otherwise, you can use Fusion360’s default values.
The Ramping Angle is depending on the hardness of the material you are milling.Here are the values we recommend:
- MDF: 15°
- Plywood: 12°
- Softwood: 10°
- Hardwood: 5-8°
- Aluminium: 1-2°
To mill pockets, you have to choose between 2 different operations (as explained before) : Pocket and Adaptive Clearing. Please refer to the previous section to learn more about these two operations.
Just as for the contour operation, we’ll start by defining the end mill end preset we want to use. We will now select the pocket we want to mill out.
As long as they are all the same depth, you can select multiple pockets in the same operation.
Similarly than for the Contour operation, we can optionally adjust the heights in the third menu tab. Also here, the fourth menu tab is only used to set step depth and stock-to-leave’s.
The fifth menu tab of this operation is quite similar to the one we have for the Contour operation, except that we have multiple options for the Ramps.
We would recommend using helix’s for all materials with the angle set to the values presented before.
The values you should change here are :
Ramp Clearance Height : 1 mm
Minimum Ramp Diameter : 0.1 mm
The only difference in parameters compared with the Pocket operation is in the fourth menu tab. The Optimum Load should always be inferior to your mill’s radius (in our case, smaller than 4 mm). A higher value would cause the mill to heathen up more quickly, and a lower value would give it more time to cool down, but would also increase the milling time.
The main advantage of Adaptive Clearing over Pocket is that you can increase the depth of cut. Where we used 3.5 mm for our cut depth when setting up the Pocket operation, we will now go up to 6 mm depth. Which will greatly decrease the milling time.
There are no parameters to edit when using the Bore operation. Simply select the right tool, preset and the holes you want to bore out,
As always, you can (optionally) edit the heights to encounter thick stock or long end mills. There is no need to define ways of going in and out the stock as the Bore operation will describe a helix when plunging into the material.
Start by selecting the mill and the correct Feed and Speed.
While the Scallop operations works with any end mill, we recommend using ball nose end mills to achieve best results.
In the second tab, you have the following fields to edit:
Machining Boundary: Silhouette -> Bounding box
Additional Offset (optional) : Play a little with this parameter to make sure the end mill runs a bit outside the model, this makes sure that all of your model will be milled.
Model: Select the model you want to use the Scallop operation on.
As always, the third menu tab (Heights) is optional.
In the fourth menu tab, you will find the most important parameter for this operation: the Stepover.
The Stepover value is what defines the distance between two toolpath lines. The smaller, the more precise your 3D texture will be. But the longer it is going to take to execute the operation…
Usually, a Stepover of 0.3 mm gives good results while remaining fast enough. If it is just to rough out the profile of your model, a Stepover of 0.5-1 mm will be faster and leave an ‘OK’ result.
For very precise work on material that easily scratches (plastics for example) a Stepover of 0.1 mm might be necessary.
Please refer to our article Branding your project to learn all about the Engrave operation.
To set up a Face operation, start by selecting the tool and according Feed and Speed. In the second menu tab, select the contour of the face you want to mill flat.
In the fourth menu tab, edit the following parameters:
Stock Offset = ½ tool diameter
Step over: between 0.1 mm and the diameter of your tool. We recommend setting it to the radius of your tool.
In the last menu tab, only change the Transition Type from “Smooth” to “Straight Line”.
Mekanika is a Belgian startup based in Brussels whose ambition is to make local production more accessible. We produce desktop machines for screen printing and CNC milling, which have been recognized for their quality and ease of use, with open source plans allowing makers to adapt their tools to their specific needs.