loading
Intermediate 5-Axis Simultaneous
FeatureCAM Ultimate Class
Enroll
Lesson 2: Intermediate 5-Axis Simultaneous
Ask a Question

In this second lesson, we will program another 5-axis simultaneous milling part, further exploring FeatureCAM's 5-axis machining capabilities. Like any other part in FeatureCAM, we will utilize 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 Ultimate_2_Part.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
  • Align the X direction
  • Select a simple block stock material computed from size
  • Place the Setup in the center of the stock
  • 5th Axis Positioning

Now that we have gone through the familiar process off importing and setting up our solid model, let's import a model to be used to define our stock material, as if we are machining a part that has already been through an operation on a lathe.

  • Import Ultimate_2_Stock.x_t
  • Use the same alignment as last import

With our stock solid model imported, we simply need to apply this model to the Stock section of FeaturCAM

  • Select Ultimate_2_Stock.x_t as Stock Solid
    • Open the Stock Properties dialog
    • User-Defined
    • Stock Solid
    • Select the model we imported to define the stock
    • Hide the stock solid

Now that we have completely worked through the import wizard, and defined our stock, we have just a few short steps left before we start programming features.

  • Select the Basic tool crib
  • Select the 5_Axis.cnc post-processor

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


Create Features

  • Create a Z-Level Roughing operation to rough the part
    • Surface Milling
    • Select the entire model
    • Choose a single operation
    • Z-Level Rough
  • Create Z-Level Finishing operation with a 0.25" Ball End Mill
    • Surface Milling
    • Select all the surfaces in one of the three recessed triangular areas
    • Choose a single operation
    • Z-Level Finish
    • Cut select surfaces
    • 0.25" Ball End Mill


Simulate, Revise

  • Run a 3D Simulation
  • Run a Machine Simulation

It looks like we have a few issues to correct with our toolpath. First, we obviously have a gouge, and will need to add some multi-axis control to avoid any collisions. It also seems that our cutter is cutting past the edges we specified.

  • Add a Check Surface to help limit the toolpath
    • Srf_mill2 Properties
    • Dimensions
    • Check Surfaces
    • Add the top surface of the part

In the past, we have looked at controlling our axes using the 'Fixed', 'Lead and Lean', and 'Automatic Tilting' options. For this lesson, we are going to take a look at the remaining options found under the 'Other' header in the 5-Axis tab. Specifically, 'From Point', and 'To Point'.

From Point - This option aligns the tip of the tool away from a fixed point, The angle of the tool is constantly changing. The tip of the tool moves significantly while the head of the machine tool stays relatively still.

http://help.autodesk.com/cloudhelp/2018/ENU/FCAM/images/GUID-93DA850A-2DA5-4572-9148-0B9DFE406F69.png

To Point - This option aligns the tip of the tool towards a point. The angle of the tool is constantly changing. The head of the machine tool moves significantly while the tip of the tool stays relatively still.

http://help.autodesk.com/cloudhelp/2018/ENU/FCAM/images/GUID-6E69E27F-C45D-4207-9184-6367FE25BA25.png

  • Alter the Z-Level Finish toolpath to use the 'From Point' multi-axis option
    • Create a point at (-1.5,0,0)
    • Srf_mill2 Properties
    • 5-Axis Tab
    • From Point
    • Select the point just created
    • Reduce the z-increment (stepdown) to 0.01"
  • Run a Machine Simulation

  • Use 'Interleave spiral paths' to ensure toolpath is generated on the flat surfaces
    • Srf_mill2 Properties
    • Z-Level Strategy
    • Check 'Interleave spiral paths'
  • Run a Machine Simulation

Now that we have fixed any glaring errors with the toolpath, and explore the 'From Point' option, let's take a look at the inverse of 'From Point' - 'To Point'.

  • Alter the Z-Level Finish toolpath to use the 'From Point' multi-axis option
    • Create a point at the center of the bottom surface of the solid (0,0,-2.1)
    • Srf_mill2 Properties
    • 5-Axis Tab
    • To Point
    • Select the point just created
    • Reduce the z-increment (stepdown) to 0.01"
  • Run a Machine Simulation

We can see that we are able to achieve a very similar result using the 'From' method instead in this case. The remaining 'To and From' methods all operate the same, only they reference lines or curves instead of points.


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.

CLASS PROJECT

Share a photo of your finished project with the class!

Nice work! You've completed the class project