FeatureCAM Standard Class

Introduction: Introduction to 3D Milling

In this final lesson, we will take an introductory look at some of FeatureCAM's 3D Milling strategies, while still reinforcing what we've learning about 2.5D milling so far. As always, we will use the same workflow to help guide us through the programming of this part.

Import, Stock, Machining Prep

  • 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 standard_3.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 center of the top face 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 Mazak.cnc post-processor

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

Create Features

In this exercise, we will recognize 2.5D features from this solid model, much like we did in the previous exercise. The chief difference with this part is that we will need to machine a surface that cannot be simply defined by a 2.5D feature in FeatureCAM. Before working through these instructions, try recognizing the 2.5D features on your own! Keep in mind that there are multiple ways to program this part. Your program may very well take a different approach from these instructions, but as long as the end result is the same, it does not matter how you get there.

  • Create a Face Feature
  • Create Boss Feature
    • Boss from Curves
    • Extract with feature recognition
    • Select horizontal surface
    • Select the top of the protruding island in the middle of the part
    • Define the top as 0.00
    • Use the major part face as the bottom, as shown below

  • Create a Pocket Feature

While FeatureCAM wasn't able to automatically find all of the pockets on this part, it was able to find the pocket with the island in the middle, along with the two semi-circle pockets for us.

  • Create pocket features to machine the remaining triangular pockets
    • Use side surfaces

  • Create a Side Feature to machine the four open profiles, and two pockets running along the length of the part
    • Side from Curves
    • Extract with feature recognition
    • Automatic recognition
    • Select the four open profiles
    • Select the two long 'pockets'

  • Create hole features
    • Hole from dimensions
    • Extract with feature recognition
    • Recognize and construct multiple holes
    • Select all

Now that we have recognized and programmed all the 2.5D features on this solid model, we are ready to program the remaining face of this part using a Surface Milling feature.

  • Create a Surface Milling feature
    • Select the angled face and the end of the part
    • Choose rough, semi-finish, and finish operations to completely machine this feature
    • Rough
      • Tool Diameter: 0.5"
      • Finish Allowance: 0.01"
      • Z Level Rough
      • 3D Pocket
    • Semi-Finish
      • None
    • Finish
      • Parallel

We have now created all the features necessary for the machining of this model. It's time to check our results, and make any necessary revisions!

Simulate, Revise

  • Run a Centerline Simulation
  • Run a 3D Simulation

We will likely want to change our finish allowance for each 2.5D feature like we did in the previous exercise, however, rather than making the same edit multiple times, let's explore making global changes for a given document.

  • Change the finish allowance for the 2.5D features to 0.01"
    • Open the Machining Attributes
    • Navigate to the Mill > Stepover
    • Change the Allowance in the Finish Pass section to 0.01"
  • Open a few of the 2.5D features, and notice that the Finish Allowance has been changed for each feature

We just utilized the Machining Attributes to make a global change in our document. It is important to realize that FeatureCAM's 'built-in intelligence and automation' comes from our machining attributes. Any default behavior that we do not specifically define at the time of feature creation is being taken from our Machining Attributes. It is also important to understand the difference between Machining Attributes, and Machining Configurations. Anything we change in the Machining will only affect the open document. If you would like to make a change to the default behavior of every document, you will need to create a new Machining Configuration and set it as your initial configuration when opening a new document. It is common practice to create multiple configurations for various materials, machines, or operators, as not every material, machine, or operator requires the same machining behavior.

Explore the Machining Attributes, and make any changes to the default Machining Attributes you desire, noting how the changes are reflected in the attributes of each individual feature.

  • Once you have made any desired changes, open the Machining Configurations page
    • Create a new configuration from this document's Machining Attributes
    • Select New
    • Name your new configuration (ex. My Default Aluminum Configuration)
    • Copy settings from the open document (ex. standard_3.fm (f))
    • OK
    • Select your newly created configuration as the 'Initial configuration for new documents'

We have now essentially created a template of our machining attribute preferences, and told FeatureCAM to always use this configuration for new documents. It is a good idea to spend the time customizing your Machining Configuration early on. This will end up saving you a lot of time in the future when you are in the 'Simulate, Revise' stage of programming.

Run a final simulation

NC Code

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.