Lesson 2 - Simulate, Revise

00:09

All of our features are now created and we are ready to simulate.

00:13

Start by selecting a centerline simulation from the simulation mode drop-down and press "Play".

00:21

So it appears that FeatureCAM is returning an error and won't let us run our simulation.

00:27

We can see from the operational list in the Results tab on the right, that FeatureCAM was unable to select a tool with which to machine this bore feature.

00:37

Remember, FeatureCAM is looking in the tool crib we have selected

00:41

and has been unable to find a bore tool with the correct orientation for the sub-spindle.

00:47

Throughout this class, we've referenced FeatureCAM’s built-in intelligence and automation multiple times.

00:56

Each time we created a new feature, various feature attributes such as depth of cut, finish allowance, or lead in or lead out behavior have been populated by default.

01:08

However, we retain complete control over this behavior and all of it can be fully customized to our liking in the machine attributes page.

01:19

At the moment, FeatureCAM will only use tools in one specific orientation.

01:25

But we can change this with the Automatic Tool Orientation settings.

01:31

Open the machine attributes page in our Part View, navigate to the Miscellaneous tab of the machining attributes page and check automatic tool orientation.

01:43

This option tells FeatureCAM to first look for a tool that is the right size to machine our feature

01:49

and then automatically orient the tool to machine a given operation.

01:55

So now, as we press "OK" to exit the machining attributes page, we can see that FeatureCAM has grabbed the 6 millimeter bore bar we made in the previous lesson and automatically oriented it to machine our sub-spindle bore operation.

02:12

We can now run a 3D simulation.

02:15

Rather than quickly playing through the entire simulation, let's move the simulation speed slider all the way to the left and select "Play to next operation" as opposed to play.

02:28

This option allows us to view each operation one at a time and automatically pauses after each.

02:35

Our face operation looks great, but notice how our turn operation doesn't quite remove all the material on the sloped back end of the part.

02:45

With an 80 degree tool, there's really no way for us to effectively machine that backside from the main spindle.

02:53

When we first examine the part, we noted these undercuts, which is why we created the two turn operations earlier.

03:01

We can now edit those features so that they only machine the part of the model that we want them to.

03:08

In the last lesson, we altered our curve to extend our toolpath.

03:13

We could follow the same steps to shorten our curve.

03:16

However, there is also an easier option.

03:20

Open the turn 1 properties page, select the roughing operation, and navigate to the turning attributes tab.

03:28

Here you'll notice a few boundary options.

03:31

These options allow us to limit the area within which toolpath is generated.

03:37

In this case, we want to limit the spindle end of our boundary.

03:41

So let's set our spindle side boundary to about negative 20 millimeters.

03:47

Once we've typed that in, we can set the value, "Apply" it to the feature, and press "OK" to exit the turn properties window.

03:57

Now that we've limited our first turn feature, let's do the same with our sub-spindle turn feature to make our toolpath as efficient as possible.

04:06

Open turn 2 and once again navigate to the turning tab in the roughing operation.

04:12

Since we have transferred our part of the sub-spindle at this point, we’ll want to limit our toolpath on the spindle side again, which just happens to be the sub-spindle in this case.

04:24

Set the value to negative 32 millimeters this time, "Apply" that to the feature and select "OK".

04:32

Now as we've run a centerline simulation, we can see the change in our toolpath.

04:40

Before we exit the simulation, zoom in on the groove features and select turn 1 from the operations list to only show the toolpath for that feature.

04:50

Notice how our turning tool attempts to dip into these grooves, even though we machine them separately later on.

04:58

This isn't very efficient and it will be best if we could keep FeatureCAM from attempting to machine these grooves with our turn feature all together.

05:07

Reopen the turn 1 properties page and go back to the Turning tab on the roughing operation.

05:13

On the right, we can see an option titled Adjusted to tool geometry.

05:18

This option tells FeatureCAM to attempt to remove as much material as possible without gouging our tool into the part.

05:27

However, in this case, we are machining these grooves later on, and can avoid these sections altogether.

05:34

To do this, change the drop-down menu from Adjust to tool geometry to Remove all undercuts.

05:41

Now as we apply this change and rerun our centerline simulation, we can see that FeatureCAM avoids these areas all together with our turning feature.

05:51

It's not a huge change, but if this were a production part, it could end up saving us a lot of money in the long run.

05:59

As you may recall from my last lesson, we made a change to the depth of cut of our bore operation.

06:06

To this part, I'd like to make a similar change, but this time to every operation in this program.

06:13

Recall at the beginning of this video, we opened the machining attributes page from our Part View and altered FeatureCAM’s default behavior regarding tool orientation.

06:24

As we mentioned earlier, all default behavior in FeatureCAM comes from our machining attributes and is fully customizable.

06:32

So let's open the machining attributes window and navigate to the Turn Bore tab.

06:38

You may recognize some of the parameters here from the individual feature properties window.

06:44

Finish allowance, depth of cut, withdraw angles, all default feature properties come from this window.

06:52

Change the depth of cut to 0.8 millimeters and the Z finish allowance to 0.05 millimeters.

06:59

With those values indicated, we can press "OK".

07:03

And now as we open up each of our existing features, we can see that the depth of cut and finish allowance have been changed.

07:12

Not only were we able to alter all our programs features at once, but now any new feature we create will use these new values, too.

07:22

It's important to understand that while FeatureCAM’s built-in intelligence and automation makes the programming process quick and efficient, we don't lose any control of our final toolpath and we can still fully customize how FeatureCAM defines our new features as we create them.

07:41

Machining attributes only affect the current document.

07:45

If we would like to make changes to the attributes of new documents moving forward, we will want to save these attributes as a new configuration.

07:55

You may recall that in the first step of our workflow, we defined My Configuration as the configuration we would like to use for our new document.

08:04

To ensure that all new documents use 0.8 millimeters and 0.05 millimeters as the default depth of cut and Z finish allowance values, we can save this document's attributes as a new configuration.

08:19

Double click on machining configurations in the Part View, name it New training configuration, and indicate that we would like to copy the attributes from our current document.

08:30

Now, when we're creating new documents, we can simply select new training configuration on the new document page to use these new depth of cut and finish allowance values as our defaults.

08:44

If at any point, we would like to edit the attributes of a configuration, we can select Edit, and you'll see that the configurations attributes page opens up and we can make any changes we would like.

08:57

There are a lot of parameters throughout this page and I strongly encourage you to take the time to explore and familiarize yourself with the various attributes that you can customize.

09:09

As always, if you are unclear on what anything is, don't hesitate to open up the Help file.

09:17

With that, let's run a final simulation before moving on to the last step in our workflow, NC Code.