Lesson 1 - Create Features

00:11

With our setup finished, we're now ready to start programming features.

00:15

Using features, we essentially describe our end product, and then allow FeatureCAM's built-in intelligence and automation to handle the repetitive tasks typically associated with CAM software on our behalf.

00:31

We'll be taking a more in-depth look at how that works as we progress through this class.

00:36

In this lesson, we'll be working from an engineering drawing

00:40

to create our features by using two of FeatureCAM's feature creation methods, Features from Curves and Features from Dimensions.

00:50

You can find the drawing as well as download links for all the files you'll need to complete this lesson on the course page.

00:57

Before we start, let's examine our engineering drawing and identify the features that we'll need to create.

01:05

But to start, we're going to want to machine the overall shape of the part.

01:10

We will need to both turn the outer profile of this part and bore the inner profile.

01:16

We can then machine the groove on the outer diameter of our part and finally create the thread.

01:23

To machine our outer and inner diameter profiles, we're going to utilize FeatureCAM's Features from Curves functionality.

01:31

Features from Curves requires us to first define a profile

01:36

either by pulling it from a CAD model or sketching it using FeatureCAM's geometry constructed tools.

01:43

We are working from a drawing, so let's head to the geometry constructed tools, which can be found in one of two places, the geometry drop-down menu in the Create section of the Home tab in our ribbon or the geometry section in the Construct top of our ribbon.

02:01

These tools allow us to sketch points, lines, circles, fillets, and arcs, as well as providing some editing and dimensioning tools.

02:11

To start, let's define the outer profile of our turning feature. To sketch this, we'll use the connected line constructor.

02:20

As we select the constructor, you might notice a couple of changes to our interface.

02:25

First, our cursor has changed when we hover over the graphics area.

02:30

This indicates that we can manually pick the points to define our connected line.

02:35

Second, we can see that our assistance bar below the graphics window has changed.

02:41

Here, if we'd like to be more precise with our geometry construction, we can enter exact dimensions to define our geometry, which is what we're going to do in this case.

02:53

We'll start by defining the first point of our line at 30 millimeters in diameter and 0 in the Z.

02:60

These values are based on the setup or touch-off point location that we defined earlier.

03:06

Notice that we're entering diameter and Z values, as opposed to X and Z or radius and Z values.

03:13

This allows us to enter our values exactly as they're shown on our drawing.

03:18

We can always change this input in the dialog settings, if we want.

03:23

Now as we enter the next point of our line at 30 millimeters in diameter, and 28.4 millimeters in the Z and select Create, we can see that we've created the first segment of our connected line.

03:37

Continue entering end point dimensions for our connected line based on the dimensions specified in our drawing.

03:44

You'll notice that in addition to defining X and Z coordinates, we also have the option to define line segments by an angle and the length.

03:54

Once we finish creating geometry, we can hit the Escape key to exit out of the connected line constructor.

04:01

And next, let's create the profile defining our ID bore feature.

04:07

This time, select the two points line constructor and enter in the dimensions as shown in the drawing.

04:13

Our first point is at 18 millimeters and 0 and our second is at 18 and 50 millimeters.

04:21

The last remaining feature we want to create from curves is the outer diameter groove shown in our drawing.

04:28

Just like our outer diameter turn profile, let's use the connected line constructor to define the profile of this groove.

04:38

With the geometry defining our machining profiles finished, we need to turn each series of lines into a single profile known as a curve, which we can then use to create features.

04:51

To do this, we'll look to the right of our geometry section in our Construct tab

04:56

and here we can select the pick pieces option in the chaining portion of our Curve section.

05:02

Now we can give the curve a name in the assistance bar and manually select the segments we would like to chain together in the graphics window, paying attention to the bold blue preview of our curve.

05:15

Once we've successfully selected the entire profile, we can select Create and continue the process for our bore and groove profiles.

05:26

It's worth saying too that if at any point you make a mistake, you can use the clear pieces option to start over.

05:36

With all the profiles we're going to use chained together as curves, we can create a turning, boring, and groove features.

05:45

Like our geometry constructors, the new feature wizard can be found in more than one place.

05:51

If we navigate to the Features and Manufacturing tab, you'll notice that we have several different options to create features from curves, or we can navigate back to the Home tab and select Features in the part program section.

06:05

The feature wizard provides us with numerous options to create new features.

06:10

We can create features from dimensions, features from curves, or even new features based on previous features.

06:18

Select Turn in the Form Curve section and the next move through the wizard.

06:23

Like the stock wizard, the new feature wizard helps walk us through the creation of our toolpath.

06:29

First, indicate that we would like to use the turn profile we just created to define this toolpath.

06:36

Next, we can indicate whether we would like to offset our curve in the Z direction.

06:41

We'll leave this as 0 for now.

06:44

On the strategies page, we are able to dictate exactly how we would like the feature to be machined.

06:50

We can change the cycle type, type of toolpath, and indicate how we would like to both rough and finish the feature.

06:58

For now let's leave all these options as default.

07:01

And on the next page, we're given a summary of the toolpath we just created.

07:09

Based on the features we've described, FeatureCAM has successfully created both the roughing and finishing operation, assigned a tool for each, and indicated feeds and speeds.

07:20

These are based on our features dimensions and also the material we chose for our stock.

07:27

Next, let's follow the same process to create our boring feature.

07:31

Open the new feature wizard, select Bore from Curves, select the Bore Curve, and this time on the strategies page, let's make a slight change.

07:42

We need to provide some clearance so that we don't gouge our part.

07:46

To do this, we can check pre drill.

07:49

You'll notice how the text for the diameter and depth fields is blue.

07:54

Whenever you see this, it means that we can manually select a value in the graphics window.

07:59

So for the depth, select the blue depth text and click on each end of our boring curve to pull the length directly from our model.

08:09

Enter a diameter of 15 millimeters and press "Next".

08:13

And we can see that FeatureCAM has automatically created the entire pre drill operation for us, selecting an appropriate tool and indicating feeds and speeds.

08:23

With our turn and bore operations created, let's quickly create our outer diameter groove, leaving all the values as default.

08:34

Now with all of our features from curves created, let's create the thread feature, this time utilizing the features from Dimensions option.

08:46

Open the new feature wizard and select the thread option in the from dimension section.

08:51

As we press "Next", notice that we're met with a dimensions page rather than the curves page.

08:57

Here we can describe the feature directly instead of selecting a curve to define our features by.

09:04

Go ahead and select the thread size from FeatureCAM's default list of standard thread sizes and a thread length of 20 millimeters.

09:13

Finally, on the strategy page, let's add relief groove with a width of 4 millimeters and a depth of 1.5 millimeters.

09:22

Add a chamfer with a depth of 1.5 millimeters and tick the box to add a finish pass before pressing "Finish" to close the new feature wizard.

09:33

Before we move on to simulating our features in the next section, let's create a face feature to face off the front of our stock.

09:42

To do this, open the new feature wizard and select face from dimensions.

09:47

On the Dimensions page, notice that FeatureCAM has picked up on the correct outer diameter, inner diameter and thickness of our face feature.

09:56

As you may recall, we offset our setup by 0.75 millimeters from the face of our stock.

10:03

This is where FeatureCAM has pulled the 0.75 millimeter thickness value from.

10:09

We can leave our Z feature location at 0.

10:12

This way, FeatureCAM will start machining at Z equals 0.75 millimeters and finish facing where our turn operation starts at Z equals 0.

10:24

Notice how FeatureCAM has placed this face operation at the beginning of our machining process.

10:30

This is another great example of FeatureCAM's built-in intelligence.

10:34

Even though we created our face feature last, FeatureCAM recognizes that you generally want to face your part first, and therefore placed it at the beginning of our operation list.

10:46

With that, let's finish this feature and we have finished all the features necessary to machine our part.

10:53

This section contained a lot of information, so I highly recommend that before moving on, you go back and try to program these features again on your own.

11:03

Once you're comfortable with all the information covered in this section, feel free to move on to the next section, where we'll simulate and revise our features.