Learn more about our amazing community, what they do and why they are giving Fusion…
Automating hole recognition and drilling in Fusion 360
Regardless of whether you’re machining a simple bracket, or programming a complex injection mold core block, the chances are you regularly need to produce NC code to machine holes – probably lots of them. The act of drilling a hole into a part is arguably one of the simplest things your CNC machine is ever going to do. Programming the holes, however, can be a very repetitive and time-consuming task.
In this blog, we’re going to discuss the new hole recognition capabilities inside the Fusion 360 manufacturing extension and explain how they can help automate one of the most common programming tasks in your machine shop.
We’ll be using this mold core block as an example.
We can see that this part contains a mixture of hole sizes, hole types and hole orientations. Some can be produced with a simple drilling cycle while others are more complex, requiring combinations of drilling, tapping, and counterboring. Many holes are aligned with the Z-axis of the machine, but there are also holes aligned with the X and Y axes.
The point here is that while a hole is a simple piece of geometry, parts can often include a plethora of different hole combinations. It’s this, almost unlimited combination of hole types, that makes programming them a real challenge, especially when dealing with parts containing many hundreds, or even thousands, of holes.
Hole drilling – it all begins with feature recognition
Hole Recognition is intended to be used when programming parts with multiple hole configurations. The customary way of programming these parts is to create an operation for each section of the hole; if you think of a tapped hole for example, you would typically create three drilling operations:
• Spot drill
• Tap drill
You would then need to repeat these same operations for other sizes of tapped holes on your part. If you have, say, three sizes of tapped holes, you will need to create nine operations to complete the programming of all the holes.
Hole Recognition allows you to create general hole making templates that define the way you want to machine a hole, then use those templates to recognize hole groups. Once you’ve selected that template as your drilling action, hole recognition will create the operations to machine the selected holes, pick appropriate tools from a selected tool library, and re-order operations to minimize tool changes.
The hole drilling commands can be accessed via the new Hole Recognition option, located under the Drilling drop down menu.
When the Hole Recognition command is triggered, Fusion 360 analyzes the CAD model and identifies any cylindrical/conical holes. Once the analysis has completed a new menu is displayed to offer additional control of the drilling process.
This menu displays a list of the identified holes in the “Hole Groups” tab. It also displays additional information about the hole(s) such as the dimensions and machining setup. A fly-out menu displays an additional visualization of the individual elements that make up the hole. The interactive display helps here – as the hole groups are selected in the menu, the relevant parts of the model change color.
By default, any holes with the same dimensions are automatically grouped together. This helps optimize the subsequent drilling toolpaths as the group can be machined as a whole, and not as separate features.
The next step is to decide what to do with the identified holes. Here, we can choose an appropriate “Action” from a simple drop-down menu. Fusion 360 comes pre-loaded with some standard options including “Simple Drill”, “Countersink Drill”, and “Ignore”. The expectation is that users will build their own library of actions to define how specific hole types should be machined. These templates can be saved to a library and used on future projects for major time savings.
The Hole Groups menu also provides additional controls, such as the ability to:
• Add/remove holes to/from the calculation
• Explode hole groups – Converts the hole group into separate holes
• Delete top segment – Removes the top segment from a multi cylinder, concentric hole
• Delete bottom segment – Removes the bottom segment from a multi cylinder, concentric hole
• Split hole signature – Divides a thru hole into 2 pieces, used when machining from opposite sides
• Flip hole – Changes the machining plane to the opposite side
Choosing the right tool for the job
Once the appropriate actions have been selected, it’s necessary to decide which cutting tools to use. This is a simple case of selecting the “Tool Libraries” tab and activating your preferred tool library. Fusion 360 will then choose the most appropriate cutting tool based on some key tool specific settings.
Those new to Fusion 360 will appreciate the fact that it comes pre-loaded with a number of standard libraries. Of course, the real beauty here is the ability for you to build your own library containing your favorite tools.
Advanced options that make a big difference
Before we look at the toolpaths that Fusion 360 creates, it’s worth discussing some of the more advanced settings that can be accessed via the “Options” tab. These really can make a big difference to machine utilization and overall machining cycle times.
Hide and ignore hole groups not aligned with this setup
When active, this option limits the hole search process to identify only those holes that can be drilled using 3-axis machining in the plane of the active Setup. In this example, switching this option on means that the holes on the side wall of the part will be ignored.
Switching this option off results in Fusion 360 producing toolpaths for all holes in all orientations.
Minimize tool changes
Switching this option on, changes the order of the toolpaths to minimize the number of tool changes. If the same tool can be used on two different hole groups, those groups should be output consecutively to have the desired effect. Deactivating this option causes Fusion 360 to group machining operations by hole. Note this option is only available when “Organize each group’s operations inside a folder” is switched off.
Organize each hold group’s operations inside a folder
When activated, this setting creates additional folders with names that match the name of the hole groups and then places the resulting toolpaths in these folders. This option is only available when the “Minimize Tool Changes” option is deactivated.
Hide and ignore groups with diameters greater than:
As the name suggests, this option provides additional control over the size of holes that will be identified and machined by Fusion 360. Any holes with a diameter larger than the user defined value will be ignored.
Show only groups with an angle between:
This option can be used to limit the machining of holes, based on the angle of the hole relative to the plane of the active Setup. The option uses “Minimum” and “Maximum” angular values to prevent holes from being machined.
As an example, think about a golf ball sat on a golf tee. Let’s imagine that each dimple on the ball represents a hole that needs to be drilled into the ball. If we entered a minimum value of 0, and a maximum value of 45, we are limiting the machining to the top 45 degrees of the ball. If we changed the maximum value to 90 degrees, we are effectively allowing the entire top hemisphere of dimples to be machined.
Allows users to select the location of their preferred hole group template file.
And now the magic happens
Once all the appropriate options have been defined, it’s a simple case of clicking “OK”. Fusion 360 chooses appropriate tools for the holes and calculates a series of named toolpaths that are placed in appropriate folders within the browser.
It’s now a simple case of simulating the toolpaths to confirm all is well, before outputting them as post-processed G-code to run on your CNC machine tool.
Fusion 360 manufacturing extension available now
The addition of Hole Recognition to the Fusion 360 manufacturing extension, looks set to greatly reduce the time and effort needed to program holes on parts. Automating the identification of families of similar hole types and subsequent toolpath calculation, should convert this traditionally tedious process into big productivity gains.
Give it a try today in Fusion 360. Visit the Fusion 360 online help site for more details about the manufacturing extension.