Specifying the work coordinate system

00:08

A CAM setup defines what you want to machine and how.

00:15

Often when working with lathe parts that also include milling,

00:18

the CAM setup parameters must be set up differently than typical turning parameters.

00:25

Open the file Spun Profile.f3d.

00:31

With the exercise file open, in the Manufacture workspace, in the Turning tab, click Setup.

00:38

The Setup dialog displays, and, in the canvas, the stock appears around the model.

00:45

Ensure that under Setup, Operation Type is set to Turning or mill/turn.

00:53

This determines the available toolpaths for standard 2-axis lathes and includes settings for multi-spindle lathes.

01:03

Next, it is important to set up the Work Coordinate System.

01:07

The Work Coordinate System sets the working ZX cutting plane and the Z spindle axis orientation.

01:16

The Z is almost always on the centerline of the part,

01:20

and should point away from the chuck or clamping side of the part.

01:25

For this example, flip the Z axis 180 degrees by checking Flip Z Axis.

01:34

Next, under Model, you can select the body to machine.

01:39

By default, all models are selected.

01:43

Next to Model, click the selection tool.

01:47

Then, in the canvas, select the part to be machined.

01:52

Once you select it, the stock adjusts.

01:56

Now, under Safe Z, you can set the Z retract position, which is positioned at the start or end of a toolpath.

02:07

You can set the reference position to either the Work Coordinate System Origin or the Stock.

02:15

The Safe Z can be overridden in each toolpath operation when configuring the passes for a toolpath.

02:23

For now, leave the Safe Z Reference set to Stock front, and in the Offset field, enter, “.5”.

02:33

This allows clearance for the tool.

02:37

Under Chuck, you can specify the reference position and offset distance to the face of the chuck.

02:45

Currently, the Chuck reference is set to Model back.

02:50

In the Offset field, enter, “.75”.

02:54

Pan and zoom the model to see how the chuck repositions.

02:60

Now, open the Stock tab.

03:03

From here, you can configure the size of the stock around the model being machined.

03:09

This is important because the toolpath is calculated based on the stock size.

03:16

An accurate stock description is critical in creating optimized toolpaths.

03:22

Under Stock, the Mode is set to Fixed size cylinder,

03:26

which creates a cylindrical stock boundary that is a specific size.

03:32

To adjust this size, in the Stock Diameter field, enter, “2.75”.

03:40

In the Length field, enter, “2.5”.

03:44

Expand the Model Position drop-down and select Offset from front.

03:51

This sets the reference to the furthest Y negative position.

03:57

Then, in the Offset field, enter, “0.5”.

04:03

Click OK.

04:05

Now, it is time to apply a Turning Profile Roughing strategy.

04:11

From the ribbon, expand the Turning drop-down, and select Turning Profile Roughing.

04:19

The Profile Roughing dialog displays.

04:23

Notice that the toolpath that displays is not correct.

04:27

It does not extend out far enough, and it splits the profile in two.

04:33

This is because the X plane crosses the part and acts as the profile boundary.

04:40

To mitigate this, you must rotate the model 360° to machine all internal and external features.

04:49

Close the dialog.

04:52

To edit the setup, from the Browser, right-click Setup1 and from the shortcut menu, select Edit.

04:60

The Setup dialog displays again.

05:04

From the Setup tab, under Model, enable Spun Profile.

05:10

Spun Profile allows subsequent milling operations

05:14

and approximates a 2D profile for 2-axis turning operations.

05:20

Click OK.

05:23

Open the Turning Profile Roughing strategy again and review the model.

05:28

Notice that the toolpath now extends to the end of the part.

05:33

It also ignored the holes.

05:36

The entire profile can now be machined.