ZLevel Parameters

The information in this section will help you create and edit ZLevel operations in your Manufacturing Program.

Click ZLevel , then select the geometry to be machined .

A number of strategy parameters are available:

• in the Machining tab to define:

• the Machining tolerance,

• the Cutting mode,

• the Machining mode,

• the Pass overlap,

• and activate the  3/5-Axis Converter

• in the Axial tab:

• to define the Stepover type,

• to define the Maximum distance or the Minimum distance between pass or the Scallop height.

• in the Zone tab to define:

• the Maximum horizontal slope.

• in the HSM tab.

TSlotter tools for this operation).
Note that:

• the TSlotter tool is defined with one corner radius only, the upper corner radius being  equal to the corner radius,
• the TSlotter takes into account a 2D projection of the limiting contour:
  The limit is considered to be a prism parallel to the tool axis and passing through the limiting contour (shown in green below).
  

You can also define the feedrates and spindle speeds and transition paths in your machining operations by means of NC macros as needed.
See also macro parameters specific to ZLevel.

ZLevel: Strategy parameters

• The ZLevel strategy parameters are distributed into 3 tabs.
  By default, all 3 tabs are displayed with all their parameters.
  However, current operations only require a reduced list of those parameters.

• Click <<Less to display only those current parameters.
  The Zone tab is hidden, as well as the Pass overlap parameter in the Machining tab.

• Click More>> to re-display all parameters.

• You can also use the modal option User Interface Simplified mode in the
  Tools -> Options -> Machining -> Operation tab.

• By default, all tabs and all parameters are displayed:
  

• Click <<Less to display a reduced list of tabs and parameters:
  

ZLevel: Machining tab

• By default, or when the More>> button is pressed:
  

• When the <<Less button is pressed:
  

Machining tolerance 

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

Cutting mode

Specifies the position of the tool regarding the surface to be machined. It can be:

• Climb 
  
• Conventional
  
• Either.
  

Machining mode 

Defines the type of area to be machined:

• By plane; the whole part is machined plane by plane,
  
• Pockets only; only pockets on the part are machined,
  
• Outer part; only the outside of the part is machined,
  
• Outer part & pockets; the whole part is machined external area by external area and pocket by pocket.
  

Pass overlap

Hidden when the <<Less button is pressed.
It is the width of the overlap of the end of a pass over its beginning.

ZLevel: Axial parameters

All parameters remain displayed in the <<Less mode.

Stepover

• Constant
  
  Constant has a constant stepover distance defined in a plane and projected onto the part.
  
  You can modify:
  • the Maximum distance between passes
    
  • and the Scallop height
    

  If you enter a Scallop height, the Distance between pass is computed automatically.

• Via Scallop Height
  
  The stepover is computed from the scallop height you have set,
  within the range defined by Max. distance between pass and Min. distance between pass.
  
  All selected geometries are taken into account in the stepover computation even if these geometries are not milled.
  For example, filled holes or vertical walls outside the limiting contour influence the stepover computation and
  may generate useless paths. The by-pass consists in not selecting these useless geometries to compute the toolpath.
• Distance on contour
  
  This stepover mode completes the Via Scallop Height stepover when the part to machine results
  from a section revolution, with small structures.  

  Example: The whole part has a sharp slope but because of a small structure on one side, the Z-pitch becomes very small. It has an impact on the finishing. Distance on contour lets you select: a contour, i.e. the section of revolution by clicking the Stepover Line in the sensitive icon and using the edge selection toolbar. and a Distance On Contour which will define points on this contour, and thus a list of Z-level values.  The Z-pitches values are the Z-level values resulting from the projection of each point of the tool axis. The Min. distance between pass  value allows filtering the resulting points. It gives the minimum value between the Z-pitches values. if several points define a segment perpendicular to the Tool Axis, only 1 point is taken into account. Z-level values are ordered along the Tool Axis, and this order depends on the contour orientation. If the part is a solid of revolution, it is strongly recommended to define the contour as the half-section of the part. If the contour is the whole section of the part, most of the distance values on the Contour will double the number . Yes No

  Sometimes, the Z-level values are very close: when a mandatory plane is defined near a Z-level resulting value, when the part presents a nearly flat geometry followed by a nearly vertical geometry. Near the flat geometry, the Z-level values will be very close. In those cases, the Z-level values are automatically filtered by the tolerance value or by the Min distance between pass (when this parameter has a higher value than the tolerance). Computation is impossible: if the contour is a line perpendicular to the Tool Axis, an error message is displayed, if the contour is a closed curve and the Min distance between pass is greater than the curve length, if the projected points of the contour are not contained by the bounding box of the part, if the contour is not continuous, if the Min distance between pass  is greater than the Z-level values of the bounding box.

ZLevel: Zone parameters

This tab is hidden when the <<Less button is pressed.
It looks like this with a Conical tool:

It turns to the following when an End Mill tool is selected:

and to the following when TSlotter tool (used as an End Mill tool) is selected.

Max. horizontal slope

Maximum slope that can be considered to be horizontal (any area that is considered to be horizontal will not be machined).

• Use this parameter to define slope areas if you need a quick tool path computation.
  However, this computation may not be accurate since some parts of the tool movements may be considered
  as vertical although they are in horizontal areas.

• If you require an accurate tool path computation, we recommend that you define the slope areas with
  the Machining/Slope Area action before entering the ZLevel action.

ZLevel:High Speed Milling tab

All parameters remain displayed in the <<Less mode.

Corner radius

Defines the radius of the rounded ends of passes.
The ends are rounded to give a smoother path that is machined much faster.

ZLevel: Geometry

• Part with possible Offset on Part (double-click  the label)
• Check element with possible Offset on check (double-click  the label).
  he check is often a clamp that holds the part and therefore is not an area to be machined.

  The tool path quality is improved if check surfaces are selected.

• Area  to avoid if you do not wish to machine it (small light brown corner near the red 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,

  In standard cases, the part will be machined from the upper plane to the lower plane, i.e. from top to bottom. If you want to machine the part from the lower plane to the upper plane, simply enter the lower plane as the top plane and the upper plane as the bottom plane.

• Imposed plane that the tool must obligatorily pass through.
  Use this option if the part that you are going to machine has a particular shape (a groove or a step)
  that you want to be sure will be cut.

  To use planar surfaces of a part as imposed planes: Select the planar surfaces, Select Offset in the contextual menu and enter a value equal to the machining tolerance + the offset value on part (if any): If the machining tolerance is 0.1 mm, and there is no offset on part, you will enter 0.1 mm as offset for the imposed plane. If the machining tolerance is 0.1 mm, and the offset on part is 1 mm, you will enter 1.1 mm as offset for the imposed plane. This ensures that the imposed planar surface is respected  to within the offset and tolerance values.

• Start point(s) where the tool will start cutting. There are specific conditions for start points:

  You can select several Start points. The function tries to select a start point convenient for each set of contours (islands or pockets). if this point exists, it is used for each contour of the set. The group of areas (pockets or islands) affected by a start point are determined as follows: The nearest group of areas is affected by the Start point. In the image below, GZ1 is the nearest group. This defines a minimum distance Dmin in the image below and a first circle with a radius equal to Dmin. Let's draw a second circle with a radius equal to Dmin+Tool Diameter. All the groups at least partially located within the zone defined by those two circles are affected by the Start point. In the image below, the group GZ2 is located in that zone, thus it is affected by the Start points. GZ3 and GZ4 are not located within that zone, thus they are not affected by the Start point. There is no restriction regarding the position of the Start points selected. They can be taken anywhere, even on the part, since only the distance between the group of areas and the Start point determines whether the pocket or the island is affected by the Start point.

• Limiting contour which is the contour that defines the outer machining limit on the part.
  You can also use the Part Autolimit option, with the Side to machine, Stop position, Stop mode and Offset parameters.

  If you have selected a single face to be machined and you are not using Part autolimit, the tool will machine both sides of the face. If you use Part autolimit, the tool will stop when it reaches the edge of the face (as shown below).

If you are editing a rework or a slope area, an additional information is displayed,
ndicating which type of subset you are working on.
This field is not editable (you can not go from one subset to another).

Info

When pressed, gives the details on the parameters that were defined with the rework area.

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.

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

Please refer to the Basic Task - Selecting Geometric Components to learn how to select the geometry.