FeatureCAM Standard Class
Lesson 2: Intermediate 2.5D Milling
Ask a Question Download

Introduction: Intermediate 2.5D Milling

In this second lesson, we will import a solid model and use FeatureCAM's feature recognition to recognize 2.5D milling features from the model directly. While this part may be different from the last, as always, we will follow our defined workflow to help us program 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_2.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
    • Enter Specific Dimension:
      • Length: 8.25
      • Width: 5.25
      • Thickness: 1.05
      • Center the offsets
      • Block
  • Place the Setup in the upper-left corner of the stock and offset the Z so that the setup is even with the part face, as opposed to the stock face.

  • 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 Haas VF.cnc post-processor

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

Create Features

In the last exercise, we created features from dimensions and curves. In this exercise we will be recognizing 2.5D features directly from our model.

  • Create a Face Feature
    • No offset
  • Create a Boss Feature
    • Boss from Curve
    • Extract with feature recognition
    • Use horizontal surface
    • Select bottom surface
    • Select top and bottom
  • Create Pocket Feature
    • Pocket from Curve
    • Extract with feature recognition
    • Use horizontal surface
    • Select pocket bottom and side
  • Create Hole Features
    • Hole from Dimensions
    • Extract with feature recognition
    • Recognize and construct multiple holes
    • Select all
  • Create Side Feature
    • Side from Curves
    • Extract with feature recognition
    • Select side surfaces
    • Select the side surface defining the curved open profile on each end of the part

  • Create features to machine the two remaining features on the model using any of the methods covered so far.

At this point, we have programmed all the features necessary to machine this model accurately, and are ready to simulate our results and make any necessary revisions.

Simulate, Revise

  • Run a Centerline Simulation
  • Run a 3D Simulation

The final product seems to pass the eye-test, but let's dig a little deeper to make some revisions to how this part is machined.

  • Change the finish allowance for the boss, pocket, and all side features to 0.01"
    • Open Feature Properties
    • Navigate to the Milling tab of the Rough operation
    • Select and edit the Finish Allowance attribute
    • Set and apply changes for each feature

This is a common milling attribute that you should be aware of. By default, FeatureCAM leaves 0.05" after a roughing operation to be cleaned up by the finishing operation. For some, this may be too much material allowance, and should be taken into consideration. This would be a good point to open the 'Help' file (select help from this window) and read through the various attributes associated with each feature. Programming features in FeatureCAM is a very quick and automated process, but taking the time to dig deeper into a feature's milling attributes can save you time in the long-run as well.

  • Change the tool being used for the Boss, Pocket, and side features
    • Open the feature properties
    • Navigate to the tools tab of the finishing operation
    • Select the 0.5" End Mill
  • Review Feeds and Speeds for Face feature
    • Open face feature properties
    • Navigate to F/S tab in the finishing operation
    • Modify if desired

Here are the defaults feeds and speeds that were calculated for this operation based on the material properties of the stock material. These values are a rough approximate, and should always be double-checked. Feel free to change either the feed or speed of this operation, as well as the other operations in this feature.

  • Run a Centerline Simulation
  • Run a 3D Simulation

While we did make several revisions, as you may have expected, our simulation results were virtually unchanged. This is to be expected, as all the changes we were made were directed towards how we machined, as opposed to what we machined. While our simulation looks largely unchanged, our NC Code is certainly different. Continuing along those lines, let's look at two additional attributes: stepdown, and stepover.

  • Change the Distance Between Cuts and Rough Pass Z Increment (Stepover and Stepdown) of the Pocket Feature to 0.01"
    • Pocket properties
    • Roughing operation
    • Stepovers tab: Distance between cuts
    • Milling tab: Rough pass Z increment
  • Run a Centerline Simulation

Notice how much more toolpath has been generated to machine the pocket now. By changing these two attributes, we were able to greatly increase the toolpath density in both the XY-plane and Z-direction. Feel free to experiment with these attributes until you are happy with the results.

When adjusting your toolpath, remember that Feeds, Speeds, Stepover, and Stepdown are all related to one another. As you alter one, you will want to consider altering the others. Feel free to make changes at this point, and simulate accordingly, however, the purpose of this exercise is to simply locate and explain these attributes.

  • After making any desired revisions, 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.