|The information in this section will help you create and
edit Prismatic Roughing operations in your manufacturing program.
Select Prismatic Roughing then the geometric components to be machined.
A number of strategy parameters are available for defining:
You can also define transition paths in your machining operations by means of NC macros as needed.
Contouring pass ratio
Truncated transition paths
Not truncated: Truncated:
Fully engaged tool management
Full engagement is detected when:
It can be set to:
Stepover, which can be defined by one of the following.
Corner radius on part contouring
You can specify the following geometry:
Part with possible offset.
Rough stock is required.
Check element with possible offset. The check element is often a clamp that holds the part and therefore is not an area to be machined.
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.
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,
Imposed plane that the tool must 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.
Note that if you wish to use all of the planar surfaces in a part as imposed planes, use the Search/View contextual command to select them. When searching for planar surfaces, you can choose to find either:
To use planar surfaces as imposed planes:
This ensures that the imposed planar surface is respected to within the offset and tolerance values.
Start point where the tool will start cutting. There are specific conditions for start points:
Note that if you use a limit line or if you use an inner offset on the rough stock, the start point may be defined inside the initial rough stock. The rules concerning the domain of the contour line or the offset on the rough stock contour line above must be applied.
Whenever possible, the end of the engagement associated to the start point corresponds to the beginning of the sweeping path. If this is not possible, the path will be cut to respect the constraint imposed by the start point.
Inner points (only active if the Drilling mode has been selected in the Macro tab). There are specific conditions for inner points:
Limiting contour which defines the machining limit on the part, with the Side to machine parameter.
Automatic horizontal areas detection
When this option is inactive, the only way to ensure that a cutting plane corresponds with an horizontal area is to define an Imposed plane crossing the area. This means that you have to consider the offset on part. This plane applies to the whole part (which is not necessary). If there are several horizontal areas to consider at different levels you have to define all of the corresponding imposed planes.
Select this option to:
Then enter the value of the offset to apply on the areas (Offset on areas) and define the Maximum angle that can be considered as horizontal. The angle is measured perpendicular to the tool path.
If the machining mode is By area, the tool path will look like this:
If the machining mode is By plane, the tool path will look like this:
The cutting planes in green are the Standard roughing tool paths, the red ones are those computed for the horizontal areas detected.
The computation of horizontal areas is not possible if the part is made
of a cloud of points (STL).
Horizontal areas are always defined as pockets (no distinction outer part/pocket). You should use a limiting contour to mill Pocket only or Outer part areas.
Side to machine: Inside
Side to machine: Outside
|Note that if you are using a limiting contour, you should define the start point so as to avoid tool-material collision.|
The only supported tools are End Mills.
|In the Feeds and Speeds
tab page, you can specify feedrates for approach, 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.
Feedrate Reduction in Corners
You can reduce feedrates in corners encountered along the tool path depending on values given in the Feeds and Speeds tab page: reduction rate, maximum radius, minimum angle, and distances before and after the corner.
Feed reduction is applied to corners along the tool path whose radius is less than the Maximum radius value and whose arc angle is greater than the Minimum angle value.
When machining pockets, feedrate reduction applies to inside and outside corners for machining or finishing passes. It does not apply for macros or default linking and return motions.
Corners can be angled or rounded, and may include extra segments for HSM operations.
You can use Slowdown rate in the Feeds and Speeds tab page to reduce the current feedrate by a given percentage.
In Helical tool paths, the reduction is applied to the first channel cut.
In Back and Forth tool paths, the reduction is applied to the first channel cut and to the transitions between passes.
Combining Slowdown Rate and Feedrate Reduction in Corners
If a corner is included in a Slowdown path, the general rule is that the lowest percentage value is taken into account.
For example, if the Slowdown rate is set to 70 % and Feedrate reduction
rate in corners is set to 50%, the feedrate sequence is:
If Feedrate reduction rate in corners is then set to 75%, the feedrate
The following types of macro can be defined on a Prismatic Roughing operation:
For more information on how to save or load an existing macro, please refer to Build and use a macros catalog.
You must select one of the following approach modes to specify how the tool will engage the material:
Note that in some cases (where areas of the part are higher than the zone you are machining and when you are using a safety plane), the tool may cut into the part. In this case, deselect the Optimize retract checkbox.
These are macros that are built by the user using the elementary motions proposed in the Current Macro Toolbox. A pre-motion macro is applied between the rapid motion from safety plane and the automatic macro.
These are macros that are built by the user using the elementary motions proposed in the Current Macro Toolbox. The post-motion macro between the automatic macro and the rapid motion from safety plane.