Plunge Milling Parameters

The information in this section will help you create and edit Plunge Milling operations in your Manufacturing Program.
For more information on the operating mode, please refer to Plunge Milling.

Click Plunge Milling then the geometric components to be machined.
Only the geometry is obligatory, all of the other requirements have a default value.

Regarding the machining strategy:

Specify the tool to be used:

  • Center cutting plunger,
  • Side plunging milling cutter.

and speeds and rates .

You can also define transition paths in your machining operations by means of NC macros as needed.

Plunge Milling: Machining Strategy tab

Plunge Milling: Machining tab

Machining tolerance

Maximum allowed distance between the theoretical and computed tool path.
Consider the value to be the acceptable chord error.

Minimum plunging length

If the distance to be machined along Z on one of the point is lower than the Minimum plunging length, this point is not machined.

Plunge Milling: Axial tab

Those parameters are illustrated below:  

  • The retract motion is defined by the Lateral retract distance and the Raise distance.
  • Its direction is automatically defined by the position of the tool in the material.
  • The motion will be done insuring that the tool cannot be damaged (no machining during this motion): there is a check with the remaining material of the stock

Plunge Milling: Grid tab

Its content varies with the Grid type selected:


Only the sensitive icon below is available.

Click Points in the sensitive icon, and select the points in the 3D Viewer.
Double-click anywhere to validate the selection and revert to the dialog box.
The selection order defines the machining order.
Once the points have been selected, a contextual menu is available in the sensitive icon

or on the points

Automatic Ordering enables you to re-order all the points as shown in the dialog box that is displayed.

while Renumber changes the order of individual points.
No material check disables the material check on individual points.


A sensitive icon and one parameter are available.

Click Contours in the sensitive icon and select the contours in the 3D Viewer.
Double-click anywhere to validate the selection and revert to the dialog box.

  • The contours may be ordered or not, closed or not.
  • The contact points are computed from those contours, using the Discretization step.
  • The initial ordering of the points on a contour follows the orientation of the contour.
  • To ensure a correct ordering of the points, you can either re-order the contours, or use the Renumber contextual menu item.


A sensitive icon and several parameters are available.

Click Grid center in the sensitive icon and select the corresponding point in the 3D Viewer.

Input of Grid center is not mandatory. By default, the computation of the grid is based on the default Longitudinal direction

Starting from the Grid center, the grid is computed along a Longitudinal direction.
If necessary, click Longitudinal direction and enter the required direction in the dialog box that is displayed.

First, the tool machines a groove:

and then reaches each of the points of the grid with a constant fixed order defined by a Machining style:

When you select a One-Way Machining style, you can choose the Machining side (Left (material is on the left of the tool) or Right (material is on the right of the tool))

  • The initial drilling and first groove is not necessary for Center cutting plungers.
  • The initial drilling is not necessary for external areas.
  • You need not define a Grid center, except if you want to control the first drilling point (e.g. full material machining). If you choose to define one, it can be a point external to the grid.

The groove has a specific Groove step and a specific Groove width.
The default Groove width is the tool diameter, you can define a larger Groove width but it cannot exceed twice the tool diameter. 
In that case, the groove will be machined in Zig-zag Machining style.

The Machining style of the groove is independent from the strategy used to machine the rest of grid.

Plunge Milling: Geometry

You can specify the following geometry:

  • the Part to machine.
  • Rough stock (optional).
    • If you do not select a rough stock, the rough stock defined at the Part Operation level is taken into account to compute the material remaining  after all the operations placed before the Plunge Milling operation.
    • In Prismatic Machining, as rework is not possible, you must select a top and a bottom plane if you want to divide the machining into several operations.
    • The rough stock can only contain a plane or a planar face: the rough stock taken into account will be the material between this face and the part.
  • Offset on bottom: it is the offset on horizontal areas.
  • Offset on side: it is the offset on vertical areas
  • Check element with possible Offset on check.
    The check element is often a clamp that holds the part and therefore is not an area to be machined.
  • Area to avoid if you do not wish to machine it (the small light brown corner near the part selection area).
  • Safety plane. The safety plane is the plane that the tool will rise to at the end of the tool path in
    order to avoid collisions with the part.
    You can also define a new safety plane with the Offset option in the safety plane contextual menu.
    The new plane will be offset from the original by the distance that you enter in the dialog box
    along the normal to the safety plane.
    If the safety plane normal and the tool axis have opposed directions, the direction of the safety plane normal
    is inverted to ensure that the safety plane is not inside the part to machine.

  • Top plane which defines the highest plane that will be machined on the part,
  • Bottom plane which defines the lowest plane that will be machined on the part,
  • Limiting contour which defines the machining limit on the part.
 Please refer to the Selecting Geometric Components to learn how to select the geometry.

Appears when invalid faces have been detected.
This message disappears when you close the dialog box or when the next computation is successful.

Appears when invalid faces have been detected and when you have decided to ignore them.
This message remains displayed as a warning.

Pick the text to switch from one status to the other.

Plunge Milling: Feeds and Speeds

In the Feeds and Speeds tab page, you can specify feedrates for approach, plunge
retract, machining and finishing as well as a machining spindle speed.

Feedrates and spindle speed can be defined in linear or angular units.

A Spindle output checkbox is available for managing output of the SPINDL instruction in the generated NC data file.
If the checkbox is selected, the instruction is generated. Otherwise, it is not generated. 

Feeds and speeds of the operation can be updated automatically according to tooling data and the Rough or
Finish quality of the operation
. This is described in Update of Feeds and Speeds on Machining Operation in the NC Manufacturing Infrastructure user's guide..

Plunge Milling: Macro data

For more information on how to save or load an existing macro,
please refer to Build and use a macros catalog in the NC Manufacturing Infrastructure user's guide.

The possible Approach and Retract macros are (in Build by user mode):

  • Add Axial motion
  • Add distance along a line motion
  • Add Tangent motion
  • Add Horizontal motion

The possible Clearance macros are:

  • Optimized,
  • Along tool axis.