Creating a Sequential Groove Operation with the Legacy Interface

From the Axial Machining section, select Sequential Groove

then a position in the Manufacturing Program.

A typical part to machine with two grooves looks like this:

A Sequential Groove entity is added to the Manufacturing Program.
The Sequential Groove dialog box opens directly at the Geometry tab . This tab includes a sensitive icon to help you specify the geometry.
Areas colored red, texts such as No point and No geometrical feature has been selected indicated that geometry is required.

Still in the Geometry tab which comprises a Global and a Local tab:

In the Global tab, select the red groove depth representation then select the two holes.
See Selecting Geometry for more information.

The sensitive icon is updated with information such as the number of machining points, the depth and diameter of the first selected hole, ...
Set Number of Levels to 2.
In the Local tab, select the plane representations in the sensitive icon, and the desired planes in the part.
Plane 1 is the plane of the first groove in the part, plane 2 is the plane of the second groove.
Optional: Select the axis representation in the sensitive icon to invert the tool axis direction.
Optional: Select the check boxes below the sensitive icon to modify the corresponding data.

Select the Motions tab in the Strategy tab

and define the required motions.

Click the icon corresponding to the required motion.
Select values from the lists, or key in the values.
Click OK to add the motion.

For example:


Rank	Name	Plane number	Compensation	Feed Rate	Appl. Mode
1	Go To Plane.1	1	2	50mm_mn	-
2	Circular.1	-	-	Machining	-
3	Go To Plane.2	2	1	50mm_mn	-
4	Circular.2	-	-	Machining	-
5	Go To Clearance.1	-	1	50mm_mn	Last Level

The motions are added and listed in the dialog box.

Select the Tool tab

and choose a tool, example, a T-slotter tool with a nominal diameter lower than that of the top hole.

Drill, multi diameter drill, spot drill, center drill, countersink, tap, two sides chamfering, boring and chamfering, boring bar, reamer, T-slotter, end mill, face mill, thread mill, conical mill and counterbore mill tools are supported.

See Assigning a Tool Element to a Machining Operation.

Click More >> and select the Compensation tab to specify a second corrector.

Select the Feeds and Speeds tab

to specify the feedrates and spindle speeds for the operation.

Select the Macros tab

to specify the desired transition paths.

See Defining and Editing Macros

Click Display or Simulate to check the validity of the operation.

See Simulating the Tool Path.

The tool path is computed.
A progress indicator is displayed.
You can cancel the tool path computation at any moment before 100% completion.

Click OK to create the operation.