Preparing drilling and tapping toolpaths

00:08

When configuring drilling and tapping toolpaths,

00:12

there are several configurations available to define the drilling tool used,

00:17

the type of drilling cycle, and containment of the toolpath itself.

00:22

For this video, open the file On-Center Drilling.f3d.

00:30

In the Manufacture workspace, from the Browser, expand Setup1.

00:37

The existing toolpaths display.

00:40

Select each toolpath to quickly review it.

00:44

The model has been faced, roughed, finished, and grooved.

00:50

Now, it is time to clear the holes of the part.

00:54

Notice that there are two different types of holes in the model.

00:58

The first hole is at the center of the part, and the other three are off-center.

01:04

The lathe that will be used to drill the model in this example can only clear the hole on the centerline.

01:12

To begin, from the Toolbar, in the Turning tab, click Drill.

01:19

The Drill dialog displays.

01:23

Before selecting a tool, you must know the diameter of the hole.

01:28

In the canvas, hover your cursor over the hole,

01:31

and a tooltip displays, indicating that the diameter is 1.00 inch.

01:38

Now, back in the Drill dialog, in the Tool tab, under Tool, next to Tool, click the selection tool.

01:49

The Tool Library displays.

01:53

From the Documents library, select tool 4 1".

01:60

In the Cutting data panel, ensure that Aluminum – Drilling is selected.

02:05

Then, click Select.

02:08

Back in the Drill dialog, open the Geometry tab.

02:13

To pick the drilling location, select the face of the large, center bore.

02:19

Notice in the model that the drill point only reaches to the back face of the flange;

02:25

therefore, the drill settings need to be adjusted.

02:29

It is important to understand that drilling on a lathe is very similar to drilling on a mill.

02:36

The difference is in the way the part is held.

02:39

On a mill, it would drill from the top of the part to the bottom.

02:44

But on a lathe, the part is drilled from the front to the back.

02:50

Therefore, when configuring the drill settings, the front of the part corresponds to the top,

02:56

and the back of the part corresponds to the bottom.

02:60

Open the Heights tab.

03:03

Under Top Height, you can describe the top of the cut.

03:07

Expand the From drop-down and select Model top.

03:13

Next, under Bottom Height, ensure From is set to Hole bottom.

03:20

Then, enable Drill Tip Through Bottom.

03:24

When this is enabled, the tool drills past the bottom of the hole,

03:29

to ensure the hole is drilled all the way through.

03:33

In the Break-Through Depth field, you can specify how far past the bottom the tool should drill.

03:39

For this example, enter, “.1”.

03:44

Now, open the Cycle tab.

03:47

From here, you can select from a number of pre-defined drilling cycles.

03:53

Expand the Cycle Type drop-down and select Chip breaking – partial retract.

04:00

This drilling cycle is used for holes with depths of more than three or four times the tool diameter.

04:09

It uses multiple pecks as the tool periodically retracts

04:13

to break chips and allow coolant to enter the hole.

04:18

Click OK.

04:20

Next, verify the toolpath by simulating it.

04:24

From the Browser, select Setup1, and then,

04:29

from the Toolbar, in the Actions panel, select Simulate.

04:35

The Simulate dialog displays.

04:38

To begin the simulation from the drilling toolpath, from the Browser,

04:43

select the Chip breaking toolpath, and then, from the Simulate player, select Play.

04:51

The operation plays and shows that the area will now be successfully bored.