Basic 3D Milling

In this first lesson, we will program a simple 3D milling part, utilizing FeatureCAM's surface milling strategies. However, before we dive into our first part, we will first take another look at the workflow of programming parts in FeatureCAM. This workflow will help guide us through the programming of every part in FeatureCAM, whether it is one of the parts shown in this class, or you own part in your shop.

In this class, we will once again be following the same workflow covered in the FeatureCAM Standard class to help us program three different parts. While each part may be different, the workflow we follow to program them will remain the same. After completing this class, you will be able to use the workflow outlined in this class to tackle any project you may encounter in your shop. Whether you are programming a simple block with holes, or a complex 5-Axis part, following this workflow will help ensure you are able to complete your projects as quickly and efficiently as possible.

• Open/Import: Open a new FeatureCAM File, or import an existing solid model
• Stock: Specify size and shape of stock material you will be machining
• Machining Prep: Take into account real-world machining considerations such as touch-off points, tool cribs, and post-processors for your given machine to prepare your model for actual machining
• Create Features: Create all features needed to machine your final part
• Simulate: Simulate your toolpath to generate NC code, ensuring that your toolpath is as safe and efficient as possible
• Revise: Make any revisions necessary to further improve your toolpath, and re-simulate to verify new changes

• Open a new document, and close the stock wizard
  
  • Milling Setup
  • Inch
  • Wizard
  • My Configuration

With a blank milling document open, we can now import our solid model to program features from.

• Import premium_1.x_t

The Import Wizard will help us setup our part, covering our stock step, as well as some of our machining prep.

• Align the Z direction by picking two points along one of the part's vertical edges
• Align the X direction by picking two points along one of the part's horizontal edges
• Step through the next few windows in the import wizard to define the piece of material we will be machining this part from
  • Block
    • Compute stock size from the size of the part
• Place the Setup in the upper-left corner of the stock
• No multi-axis positioning

Now that we have completely worked through the import wizard, we are just a few short steps away from creating features.

• Select the Basic tool crib
• Select the Okuma.cnc post-processor

With our part imported, stock setup, and machining details accounted for, we are ready to start programming!

Now, with our model imported and setup, we are ready to start programming features. Immediately, it is obvious that this model cannot be defined using FeatureCAM's 2.5D features. We will need to machine this entire model using traditional surface milling strategies. Select the model surfaces by box selecting the entire model

• Create an Z-Level Roughing operation
  
  • Choose a single operation
  • Z-Level Rough
  • Offset/spiral
  • 3D Boss
• Create a Parallel Finishing operation
  • Choose a single operation
  • Parallel Finish
  • X parallel
  • Automatic
  • Use stock dimensions
  • None

• Run a Centerline Simulation
• Run a 3D Simulation

Notice the small areas not touched by the finishing operation in the lower curved corners. This is due to tool selection. By default all surface milling operations select a 0.5" end mill. This default behavior can always be changed in the Machining Attributes. In this case, the curvature of the 0.5" ball end mill is simply not small enough to machine the desired contour, and a smaller tool will be required.

• Create a new 0.25" ball end mill for the Parallel Finishing operation
  • srf_mill2
  • finish1
  • Tools tab
  • Create a new tool
  • Copy the dimensions as shown below, and activate the new tool

• Run a 3D Simulation

Now that we have fixed that issue, it's time to take a look at surface finish. Notice how the finish on the corners along the x-axis look good, but the finish along the y-axis leaves large scallops. This is because we are going an X-Parallel operation. Any surfaces where the tool is machining along the slope will look fine, but machining across slopes will leave larger scallops.

• Add a perpendicular remachining pass to the Parallel Finishing operation
  
  • srf_mill2
  • parallel
  • Strategy
  • Check 'Add perpendicular remachining pass'
• Run a 3D Simulation

Notice how much better the finish is on the corners of the model.

• Decrease the finish stepover to 0.005" to further improve surface finish, and run a 3D simulation

Notice how improved the surface finish is now! While the finish is much better, if you navigate to the details tab of the results window, you will notice that this part now takes roughly an hour to machine. You will want to consider machining time when modifying attributes such as stepover, and choose the value that best suits your project's needs (surface finish vs. time, etc.)

With our final simulation run, our NC Code has been generated and is ready to be sent to the machine.

• Select the Show NC icon to open our NC code in the Results window.
• Select the Save NC icon to save the displayed code.
• Save the NC code to your desired directory.

Note: This exercise is for educational purposes. The post-processor used in this exercise is a generic post-processor used for training that will likely not work for your machine. Do not attempt to run any code generated in this exercise.