Lesson 2 - Simulate, Revise

00:09

Now with our standard 3D surface milling features created, it's time that we simulate those features and revise them to add 5-axis simultaneous control.

00:19

So to start, let's run a machine simulation.

00:23

I'll play to the end of the roughing operation first.

00:28

Slow down the simulation slider.

00:33

And let's watch our finishing operation.

00:42

As we can see, before too long, we have a gouge in our finishing operation.

00:48

If I zoom in, we can see that this is due to the length of our tool.

00:53

Now if we were working on just a 3-axis mill, our only real option would be to grab a longer tool.

00:59

However, this can result in poor surface finish.

01:03

So, since we are working on a 5-axis mill, we will utilize FeatureCAM's 5-axis simultaneous control to maintain our tool length, and therefore, surface finish while machining this finishing operation.

01:17

So let's eject the simulation, open up our surface mill 2 feature and navigate to the Z level finish, 5-axis tab.

01:28

In the last lesson, we took a look at the fixed lead, lean and tilt axis for gouge avoidance options.

01:36

Just as a quick review, with our fixed option, we were able to define a vector that would ultimately be our tool axis vector.

01:46

Whenever we defined our vector, so for example, 0,0,1, our tool axis would be aligned with that vector at all times while machining.

01:55

The next option we looked at use lead, lean allowed us to indicate a lead angle and a lean angle, and kept our tool at those exact angles from our contact normal of the surface we were machining.

02:10

So for example, when we entered in a lead and lean angle of zero, at all times we were machining perpendicular to the surface.

02:20

Finally, in our last lesson, we took a look at the tilt axis for gouge avoidance.

02:25

This allowed us to indicate any of the above options, and in the case that we would collide, FeatureCAM would automatically lead or lean for us to avoid the collision.

02:36

In this lesson, we'll be taking a look at a few of the remaining options found here in the other section, specifically, From Point and To Point.

02:48

The From Point option allows us to align the tip of the tool away from a fixed point.

02:55

So the angle of the tool is constantly changing, while the tip of the tool will move significantly while machining the surfaces, the head of the machine tool will stay relatively still.

03:06

So with from point, we’ll define a point and at all points the head of our tool axis will travel through that point while the tip of our tool moves around to program the surfaces.

03:18

Don't worry if that didn't make sense to you.

03:20

We’ll utilize our From Point option and run a machine simulation to get a better visual representation of what I mean.

03:27

To utilize this option, first, we're going to need to create a point.

03:33

To do this, I'll navigate to our Constructs tab, select point, and I'm simply going to place one at negative 1.5 in the X, 0 in the Y, and 0 in the Z.

03:48

This is going to be the point where the head of our tool axis is always in line with.

03:53

With that point created, I’ll navigate back to the 5-axis tab of that Z level finishing operation.

04:02

Select From Point and select that point that we just created.

04:09

Now that we've given our toolpaths and 5-axis control, let's make a couple more changes.

04:14

First, go to the finishing operation, Milling tab, and let's just change our Z increment from 50 thousandths to 10 thousandths of an inch.

04:23

We’ll set that value and "Apply" it to the feature.

04:27

Also, you may have noticed in our machine simulation that it looked like our tool was traveling past the surfaces that we wanted to machine.

04:35

Specifically, it was machining this face on the part.

04:39

So to correct this, we’ll select this surface as a check surface in FeatureCAM.

04:46

Part surfaces in FeatureCAM are the surfaces that we would like to machine.

04:50

So whenever we've created a surface milling feature and pre-selected surfaces, we were selecting part surfaces.

04:57

Check surfaces or surfaces in FeatureCAM that we do not want to machine

05:01

and that will stay away from by given tolerance set in our machining attributes.

05:06

So, open up Check Surfaces, use the Pick Surface option and pick this Top surface.

05:14

This will now tell FeatureCAM do not cut near the surface with the tool.

05:20

Select "OK" and "Apply".

05:22

"OK", and let's run another machine simulation.

05:37

Now as I play the finishing toolpath, notice the change that has been made since we selected From Point.

05:44

Again, From Point aligns the head of our tool axis with the point that we've created and selected in our 5-axis tab.

05:53

We’ll expect the head of the machine to stay relatively still, while the tip of the tool moves around quite a bit to machine the surfaces.

06:20

Hopefully that helps you visualize the From Point option.

06:24

If you're still having trouble visualizing that, I'd recommend creating multiple points all around the part and selecting them as your From Point option.

06:33

The more extreme of points you create, the easier it will be to visualize.

06:38

Moving on from the From Point option, let's take a look at the inverse, the To Point option.

06:44

To Point does the exact opposite of From Point.

06:48

With From Point, the head of our tool axis was aligned with the point, while the tip was free to move around while machining.

06:56

With To Point, the tip of our tool axis will be aligned with the point while the head of our machine is free to move around.

07:03

So it's the exact opposite.

07:06

So, before we do that, let's eject the simulation and let's create the point that we would like to machine to.

07:13

Create a new point at 0 in the X, 0 in the y, and negative 2.1 in the Z.

07:23

This will create a point at the center of the bottom surface of our solid model.

07:28

So I'll select Create, reopen our surface mill 2 properties, go back to the 5-axis tab in the Z level operation, select To Point and grab that point that we just created.

07:50

Now with that new point selected, let's just make one more change to our feature.

07:54

As you may have noticed, we weren't actually machining this bottom flat surface.

07:58

So to change this, I'll go to Z level, strategy, and select Interleave spiral paths.

08:07

Basically what happened here is that our flat surface fell between two different Z level slices of our operation.

08:14

The interleave option inserts toolpath in the shallow regions between the slices.

08:20

This option attempts to finish the entire part with a minimum number of retracts.

08:25

So with that, we’ll select "Apply", "OK", and let's run another machine simulation to get a good idea of what the To Point option looks like.

08:46

Now as we finished the surfaces, notice that the tip of the tool is always aligned with that point that we created.

08:53

So now, the tip stays relatively still, while the head of our tool axis is free to move around.

09:11

Now as our simulation is finished, you can see, we were able to achieve a very similar result using the To method instead of the From method in this case.

09:21

The remaining to and from methods, all operate the same, they just use different entities to describe what the head and the tip of the tool axis are doing.

09:31

So for the From Line and To Line options, you want to create a line and select whether you'd like to go from or to that line.

09:41

Likewise, with curve, you can create any curve that you would like

09:44

and tell FeatureCAM to always have the tip or the head of your tool axis aligned with that curve.

09:51

This concludes our simulate and revise section of this lesson.

09:56

Before moving on, I strongly recommend that you try programming the rest of this part on your own.

10:03

Try programming the two remaining pockets using a variety of different options, whether it's from line, to line, from curve, to curve, or the ones we've already covered, such as fixed, lead, lean, and automatic tilt.

10:17

This part can be completely programmed using every single one of these options and this is a great opportunity for you to explore the different options and see what the strengths of each ones are.

10:27

Once you're happy with your final results, feel free to move on to the next and final section, NC Code.