This instructable will walk you through the process of taking any 3D surface made in Fusion 360 and making a 3D milling CAM setup to prepare it for a CNC machine. In the CAM workspace, we'll establish the stock (the material to be carved out) dimensions, choose a tool (an end mill in this case), enter the proper settings for cutting, and create a tool path that can be run on the Othermill.
The model used in this Instructable was made using the process I describe in this Instructable: https://www.instructables.com/id/3D-CNC-Relief-Sculpture-Fusion-360/
Step 1: Fusion 360
Autodesk Fusion 360 (Free)
This is a powerful 3D modeling platform that's easy to learn but has endless potential. With it, you can design complex 3D objects for practically any kind of fabrication, digital or otherwise.
- Follow one of the links above to download the app (don't use the App Store on Mac).
- Enter your email and download the free trial.
- Install and setup a free Autodesk ID account.
- When you open Fusion, select the Trial Counter in the upper toolbar (it tells you how many days are left on your trial).
- In the next dialog box, select "Register for Free Use".
- Sign up as a Start-Up or Enthusiast (Free). You can also Sign up as a Student or Educator (Free) if you're a student or educator at a registered institution.
- Select the "I accept Terms and Conditions" checkbox and click Submit.
Step 2: Create New CAM Setup
First, switch to the CAM workspace in the workspace drop-down list on the upper left of the interface. Next, click SETUP > New Setup. A generic stock will automatically be created and represented as a translucent box around the solid object.
The Axes will be based on the model environment in which Y is the "up" axis, but for CAM, Z has to be the "up" axis. To change the axis, just click on the arm of the Z axis arrow, then click any line in the model Y axis. You can click the arm of the Z axis, then click the up-axis on the model origin (NOTE: The model origin has to be turned on in the MODEL workspace).
The CAM origin should now be set with Z as up, X pointing to the right from this point of view, and Y pointing to the left along the base of the model. If the X or Y axes aren't pointing the right way, you can flip them by clicking the ends of the arrows.
To set the origin, you can click Origin and select Model Origin, or you can click on the origin point (white ball where X, Y, and Z meet) of the CAM axis and click again on any point on the model or on the model origin if your piece is placed on it.
The Stock tab will show a default offset in each dimension. I set all of these offsets to 0 because I don't want to leave behind any stock.
Step 3: Create New Milling Operation
With our CAM setup complete, it's time to create a milling operation. There are lots of options, but for a carved surface like this, the best results will come from 3D Pocket Clearing.
Go to 3D > Pocket Clearing in the ribbon menu.
The machining operation menu is where all the settings are entered to create the proper tool path for milling. The first item on the list is the Cutting Tool. Click the Select button and choose one from the list. The default list that's included with Fusion is a good place to start, but you can always add more tool settings and save your own when you get deeper into CNC.
I chose a 1/8" ball nose 2-flute spiral end mill, but you could cut a similar surface with lots of other types of bits. Ball Nose bits result in smoother surfaces and are often used for finishing passes after a rough cut has been done with a flat end mill. For a project this small, I don't see the need to create a rough cut first.
Step 4: Tool Settings / Feeds + Speeds
When you're running a CNC mill, it's important to have the proper settings. The basic settings can be summed up in terms of "feeds and speeds".
You will see lots of variables in the Tool tab of the Toolpath window, but I want you to pay close attention to just these two when you're getting started in CNC:
- Feedrate: The distance the spindle moves relative to the time it takes to move along the workpiece.
- Units are distance / time, usually in/min or mm/min.
- Spindle Speed: The rotational speed of the spindle.
- Units are revolutions per minute or RPM.
All of the other variables (Cutting Feedrate, Feed Per Tooth, etc.) will update automatically when you adjust these two. The goal here is to optimize the feeds and speeds so that your work is cut as quickly as possible without breaking the end mill.
If the feedrate is fast and the spindle speed is too slow, the end mill will break under the lateral pressure:
If the feedrate is slow and the spindle speed is faster than it needs to be, there will be little risk of breaking the end mill, but the job will take longer than it needs to:
What you want is the Goldilocks zone: a spindle speed fast enough to cut easily and a feedrate that's as fast as possible without risking too much lateral strain:
Of course, the hardness of the material plays a major role in the proper feeds and speeds. Metals need slower spindle speeds to avoid overheating, for example. Rigid foam is so soft that you can practically crank up the feedrate to full tilt without worrying about breaking an end mill. Soft wood will be somewhere between these two extremes.
RECOMMENDATIONS FROM OTHERMILL:
General recommendations can be found in lots of places. CNC manufacturers provide recommendations as do end mill manufacturers. If you want to dig deep, there is no shortage of feed / speed calculators out there that will help you really dial in the perfect settings. In my opinion, though, it's only really necessary to perfectly calculate all the settings if you're doing production work.
I've found that the default settings from Othermill are a good starting point.
These are their recommendations for Mahogany, which is a good bit harder on the scale than Poplar, so it's safe to assume these settings are a good place to start.
Tool: 1/8" Ball Nose Endmill
- Spindle speed: 10,000 RPM
- This is the rotational speed of the tool.
- Plunge Feedrate: 15 in/min (381 mm/min)
- This is the speed of the tool as it travels against the material. This feedrate is lower because plunging puts more stress on the material.
- Other Feedrates: 20 in/min (508 mm/min)
- The other federates are set to 20 in/min. You can get very sophisticated with these to get the best results, but this is a safe starting point.
Based on the recommendations above, here are the final Feed and Speed settings for this milling operation.
Step 5: Geometry
Next, go to the Geometry tab and click on the surface you want to mill. The tool wants you to click on the bounding edge of the surface as shown. There's no need to touch the other settings in this tab for now.
Step 6: Heights
Next, click on the Heights tab to set the vertical dimensions of the milling operation. Here's a quick rundown of what to do here:
- Clearance Height: the first height the tool rapids to on its way to the start of the tool path.
- Once the stock top and bottom are set, we'll move this manually to make sure they're not too tall for the Othermill's small Z height.
- Retract Height: the height that the tool moves up to before the next cutting pass.
- We'll also move this manually to make sure they're not too tall for the Othermill's small Z height.
- Top Height: This is what the tool path will recognize as the top plane of the model.
- To set it, select Selection under the From menu and click on one of the top corner points.
- Bottom Height: This is what the tool path will recognize as the bottom plane of the model.
- To set it, select Selection under the From menu and click on one of the bottom corner points.
Step 7: Passes
The Passes tab is where you'll set the cutting passes. The first important setting here is Tolerance, which you should set to .001. With such a small machine and a small cut, there's no need to have this setting any higher.
The second setting is Maximum Roughing Stepdown: this sets the distance the tool steps in the Z direction as it cuts.
Stepover distance is the lateral distance the cutting tool travels when it is carving a complex surface or surfacing a flat plane. When carving with a ball nose end mill, it's important to choose a stepover that leaves as little residual material (called scalloping) as possible without taking too much time.
Using the Othermill, I performed a test using a 1/8" (3mm) ball nose end mill clearing 9 squares with different stepovers, increasing from 1/2 of the tool diameter up to 1/10 of the tool diameter. As shown in the graphic below, 1/8 Ø produced the best results with the least amount of time. At 1/7, the scalloping started to be visible, but at 1/9 and 1/10, the scalloping was practically indistinguishable from the 1/8 pocket. CNC is all about optimizing for time and quality. This kind of test can save you lots of time as you use the tool more. The F3D Fusion 360 archive in this step can be used to run the same test on any machine.
Smaller stepdowns will make for smoother surfaces, but if they're too small the toolpath will take forever to cut. Here are the settings to pay attention to:
- Maximum Roughing Stepdown is where you set the stepdown for this file. In the demo, I went with 1/5 of the diameter, or .025" to save time.
- Stock to Leave should be unchecked since we don't want to leave any material. This might be useful if you intend to cut the stock off with a saw when the milling operation is done.
Step 8: Linking
Finally, click the Linking taband set Ramp Type to Profile. Hovering over this menu shows a preview of the type of operation- Profile looks like it will make smooth transitions, but some of the others might work as well.
Now click OK and take a look at your tool path.
Step 9: Toolpath Preview
Fusion will give you an animated preview of the tool path before you send anything to a CNC machine. This is great because it helps you catch errors before you cut anything.
Go to ACTIONS > Simulate and you'll get a timeline at the bottom of the screen and a control window. If you turn off Toolpath and turn on Stock, you can see a preview of the milling operation. Errors and possible collisions will show up in RED on the timeline at the bottom, so you'll be able to make changes as needed to your machining operation.
Step 10: Post Process G-Code
Now that the tool path is set up, it's time to create a gCode file (the set of instructions that the Othermill can read). Go to ACTIONS > Post Process, and select "othermill.cps - Generic Othermill" as the post processor. This will save the gCode file in a local folder where the Othermill control software can access it.