Lesson 3 - Create Features

00:08

With our part completely setup for programming, we are now ready to start creating the features necessary to machine our model.

00:17

As we discussed earlier, in this lesson, we will be combining the traditional turning features we've covered in the first two lessons of this class with FeatureCAM's milling features to fully utilize the live tooling of this turn/mill style lathe.

00:34

The key difference between a turning feature and a turn/mill feature in FeatureCAM really comes down to which components are rotating.

00:42

With a traditional turning feature, the part is rotating while the tool simply translates.

00:49

Contrast this to a milling feature, where our tool is rotating while our part stays relatively still.

00:57

Introducing milling features to our turning document opens up a lot more versatility in the parts we can program, allowing us to machine off-center features on our part.

01:09

To begin our feature creation, as always, let's create a new face feature to clean up the front face of our part.

01:16

Open the new feature wizard and indicate that we would like to create a turning as opposed to a turn/mill face feature.

01:24

Select face from dimensions and make sure that we have an OD of 240 millimeters, ID of 0, thickness of 3.25 millimeters, and location of Z equals zero.

01:37

Now with the face of our part cleaned up, let's turn the OD profile of our part before we start creating milling features.

01:45

As we've done in the past, we'll use the revolved boundary curve creation method to extract a profile to help define our turn feature.

01:55

Open the curve wizard and select revolved boundary and the curve from surface section.

02:01

Make sure that the polygonal method is selected and don't forget to check convert to geometry.

02:08

With our profile created in the form of geometry, let's chain together the curve we’ll use to define our turn feature.

02:16

To make things easier on ourselves, hide the solid before taking a side view.

02:21

Let's chain our profile starting with this horizontal segment at the front of our part, working up and back to this top horizontal segment.

02:31

Now we can name our curve and hit "Create".

02:35

At the moment, our turn feature stops partway through our stock.

02:39

Let's extend it through the back of our part in a similar way to the first lesson.

02:45

This will help ensure that we have a clean back edge when we cutoff our part.

02:51

Now with our curve created, let's create our turn feature leaving all default values and strategies.

03:06

With all of the necessary turning features created, let's create our first milling feature to machine the geared profile around the OD of our part.

03:16

Open the new feature wizard and select turn/mill.

03:20

If you look closely, you'll notice that this new feature window looks pretty different from the new feature wizard we've grown used to in this class.

03:28

All the features you see here are standard milling features in FeatureCAM.

03:33

As I mentioned before, this class is more focused on lathes and we won't be diving too deep into the details of milling features.

03:41

If you plan on programming a lot of terminal parts for your own life tooling lathe, I strongly recommend that you take a look at our FeatureCAM milling content to better familiarize yourself with the world of milling in FeatureCAM.

03:55

In this case, let's machine this profile using a side feature.

03:60

Select side in the from curve section and check the box titled Extract with Feature Recognition.

04:07

This indicates to FeatureCAM that rather than creating our own curves to define this feature, we would like FeatureCAM to automatically recognize this side feature directly from the solid model.

04:20

On the feature alignment page, select along the setup Z axis.

04:25

If our machine included a B-axis head, we could choose machine feature around our index axis as well.

04:33

With our feature alignment defined, now it's time for us to dictate how FeatureCAM should attempt to extract the side feature from this model.

04:41

We have several different manual options here that provide us with a lot of control.

04:47

However, let's simply use Automatic Recognition in this case, as this side feature is fairly straightforward.

04:54

We can now see that FeatureCAM has recognized the outer profile of our part, as well as several holes.

05:01

For now, let's just click on the blue outer profile.

05:05

As we click it, we can see that the feature turns red, indicating it has been selected.

05:12

Keep in mind that you can always re-click on a selected feature to unselect it, if needed.

05:19

At this point, we can hit "Finish" to create our side feature.

05:25

Even though we just programmed a milling feature using an entirely new method, the new feature wizard helps us break down this complex task into a series of simple questions and definitions.

05:37

Even though the process was slightly different from what we've seen up to this point in the class, creating milling features is no more difficult than creating turning features.

05:48

So now that we've milled the outer profile of our part with our side feature, let’s machine the pocket near the front of our part.

05:56

To do this, once again, let's open the new feature wizard, indicate that we'd like to create a turn/mill feature, and this time select Pocket in the from curve section.

06:07

Again, we'll make sure that extract with feature recognition is selected and press "Next".

06:14

Select along the setup Z axis and let’s attempt to use FeatureCAM’s automatic recognition again to extract this pocket feature from our model.

06:24

It looks like FeatureCAM had no problem finding this pocket feature.

06:29

Make sure to select the blue wireframe preview in the graphics window and press "Finish".

06:35

Next, we need to decide how we'd like to machine the remaining holes.

06:40

The holes around the outer edge of the part and the hole in the center are rather large, so it would probably make sense to mill these with an end mill, while the five holes in the middle of the part are a bit smaller and can probably be drilled just fine.

06:56

Let's start by milling the larger holes.

06:59

Open the new feature wizard and select turn/mill.

07:02

To machine these larger holes, let’s create pockets again, remembering to ensure that extract with feature recognition is selected.

07:11

Make sure that along the Z is selected and press "Next".

07:16

As we just saw, FeatureCAM’s automatic pocket recognition was only able to find the pocket we've just created at the front of our part, so we won't be able to extract these larger holes using the automatic recognition method.

07:29

Instead, let's use the select side surfaces method.

07:34

With this method, we can simply select the cylindrical sidewalls of each hole and add them to our feature.

07:47

Press "Next" after selecting all of our side features.

07:51

And we can see that FeatureCAM has extracted the top and bottom of our side surfaces to help define our pocket feature's depth.

07:59

FeatureCAM has pulled these values from our model.

08:02

However, if we'd like FeatureCAM to start machining higher than the top of the side surfaces or lower than the bottom, we could manually override that here.

08:12

Leave these values as they are and continue.

08:15

Here we can confirm the dimensions of our pocket.

08:18

We'll leave those as well as our milling strategies as default and confirm the roughing and finishing operations, that FeatureCAM has just created to machine these pockets.

08:30

With the pocket features created to mill our larger holes, let's drill these smaller holes near the inside of our part.

08:37

Open the new feature wizard again, select turn/mill, and this time we'll select the Hole feature option.

08:46

Make sure to indicate that we’ll be creating these holes along our Z axis.

08:51

And on the next page, we’ll notice a few new options that we haven't seen before.

08:57

Select Recognize and construct multiple holes since we'd like to create five holes in this case.

09:04

And below, check the box to exclude holes greater than a value of 25 millimeters.

09:11

This will ensure that FeatureCAM doesn't attempt to create hole features from the larger holes as well.

09:18

With that indicated, we can press "Next" and we can see that FeatureCAM has extracted the five small holes we were looking for.

09:26

Let's make sure to check the option to merge similar holes into a pattern.

09:31

And since FeatureCAM only picked up these five holes that we wanted, we can hit "Select All" and "Finish".

09:38

Notice in the Part View how FeatureCAM turned these five holes into a single hole feature that has been patterned five times.

09:47

With that, we have finished programming all the features required to machine our model.

09:53

So to wrap up our Create Features section, let's create a cutoff feature to part of our model before moving on to the simulation portion of our workflow.

10:03

Open the new feature wizard, select turning and cutoff from dimensions.

10:09

Make sure we have an OD of 240 millimeters, an ID of 0, a width of 0.75 millimeters, select a Z location and press "Finish".

10:25

With all of our features created and our part cutoff, we're now ready to move on to simulation.