Let’s hear everyone’s final project proposals. What do you plan to do? What do you need to do it?
Before we start CAM’ing
Before we start, we need to make a few adjustments to our Fusion 360 setup.
Set Z to up
On your CNC machine, most likely the Z axis is the vertical axis — the axis that typically holds the tool and goes up and down. So make it that way in Fusion too.
- Click on your name in the upper right, and then click on Preferences.
- On the “General” tab, change the default modeling orientation from “Y up” to “Z up.”
Download Tool Library
We will download the tool library for the Othermill CNC. – via
- Download the tool library and unzip it. It will contain two files: Tool Library.json for Fusion 360 users, and Tool Library.hsmlib for HSM users. (The filenames may change depending on the version of the tool library you’ve downloaded.)
- In Fusion 360, switch to the CAM workspace. Then open the Tool Library from the Manage menu in the toolbar.
- In the CAM Tool Library dialog, click the Local library, then click the Import Tool Library button in the toolbar. It’s the second button in the toolbar, with an arrow pointed downward into a box.
- Find the .json file you just downloaded and click Open. The tools should now appear in your library.
CAM on Fusion 360
You must first have a 3D model made. Then change from the Design workspace to the Manufacture workspace.
Create a New Setup
Select Machine, “Generic 3-axis”
Operation Type “Milling”
Choose “Select Z axis/plane & X axis.” Click the button next to “Z Axis” and then select a face or line on your model that’s perpendicular to the z-axis. In other words, choose a line or face that would be lying flat in the milling machine. You should see the blue z-axis indicator stick out of the face you selected, and the arrow should be pointing in the positive (or “up”) direction. If not, click the head of the arrow or check the “Flip Z Axis” checkbox to flip the orientation.
Now set the x-axis orientation following the same procedure you followed for the z-axis. If it’s already oriented correctly, you don’t need to do anything.
Set the origin. Bantam Tools software sets the origin based on the size of your material, so click the Origin menu and select “Stock box point.” Then, click the Stock Point button. A number of points will appear on your model. Click the point that represents the top, left, front of your material.
To verify your setup, look at your model from the Home view. You should see that:
- The origin is in the top, front, left corner of your model.
- The red X-axis arrow is pointing to the right.
- The Y-axis arrow is pointing away from you.
- The Z-axis is pointing upwards.
Setup Stock Material
Click the Stock tab, then click the Mode menu and select “Fixed size box.” Enter your material’s X, Y, and Z dimensions, measuring with calipers if possible. Set “Round up to Nearest” to 0.
Fusion 360 will place your model in the exact center of your stock. You may want to align your model to the surface of your stock or offset it by some absolute amount. To do this, choose the “Model Position” for the dimension you want to align to, choose the side you want to offset from, and fill in the Offset field with the amount you want to offset by. Entering 0 will align your model flush to that face of your stock.
Facing is a 2D milling operation that mills a flat face onto the material. It’s used to ensure that the material is perfectly flat, and as such, it’s often the first toolpath in a sequence. When configuring a facing toolpath, Fusion 360 will automatically mill the entire piece of material, from the top of the material to the top of the model.
To set up a 2D Face, click the 2D toolpath menu and select Face. A new panel will open and allow you to configure this toolpath. This panel has five tabs, each with a number of settings.
- Tool is for selecting a tool and specifying your feeds and speeds.
- Geometry is for selecting the geometry you wish to mill.
- Heights is for specifying vertical dimensions of the toolpath.
- Passes is for configuring the depth of passes, stepover, and stepdown.
- Linking is for specifying how the toolpath will begin and end.
We will select the 1/8″ Flat End Mill tool and leave everything else as default for now.
We can simulate the toolpath if we like.
3D Adaptive Clearing
3D Adaptive Clearing is a Fusion 360 milling strategy for roughing out large areas of material. It’s a great way to quickly set up a toolpath for a complex part and is also a good first step if you don’t know what type of toolpath to choose.
To set up a 3D Adaptive Clearing toolpath, in the 3D toolpath menu, select Adaptive Clearing.
Tool tab. We will keep the tool the same, 1/8″ FEM.
Geometry tab. Deselect Stock Contours to ensure that the toolpath mills the entire piece of stock configured. Disable Rest Machining to disregard previous toolpaths. (Rest Machining is a powerful way to combine multiple toolpaths.) Leave Tool Orientation and Model unchecked.
Leave Height tab alone for now.
Passes tab. Although there are many options on this tab, the most important are Optimal Load and Maximum Roughing Stepdown. These set the amount of material the tool will cut on each pass. Set values for both that are no more than half the diameter of your tool. You may want to reduce this value further depending on the surface finish you desire and the tool/material you’re using.
If you don’t plan to set up a separate finishing pass, uncheck Stock to Leave.
Now that you have toolpaths configured, you’re finally ready to export toolpath G-code files. For each toolpath, do the following:
- Select it in the Browser panel.
- Click the Post Process button under Actions.
- In the Post Process panel that pops up, set Post Processor to “othermill.cps – Generic Othermill (Otherplan).”
- Under Program Number, enter a number. This is a comment that will show up in the file so you can tell which order the file is supposed to be cut, just by looking at the contents of the file.
- Optional: For Program Comment, enter something descriptive. Again, it’s just a comment inside the file that you can read to determine what’s going on in the file.
- For Units, select Document Unit.
- Leave “Minimize tool changes” unchecked.
- Uncheck “Open NC file in editor,” unless you want to make manual changes to the G-code.
- Leave all the Properties values alone.
- Click OK and choose a destination to save your file, making sure that it has an .nc extension, otherwise the Bantam Tools Software won’t recognize it.
Open Toolpath in Bantam software
This is where you leave the digital and setup a physical machine. We will end here. If you are curious to try the CNCs, please let me know.
Start your final projects. Try to make progress on it for the next 3 weeks.