The information in this section will help you create and edit Trochoid Milling operations in your manufacturing program.
Select Trochoid Milling then select the geometry to be machined .
A number of strategy parameters are available for defining:
Specify the tool to be used , NC macros , and feeds and speeds as needed.
The figure below illustrates the trochoidal motion:
This motion is generated on the whole tool path while respecting:
Direction of cut
Specifies how machining is to be done.
Climb milling, the front of the advancing tool (in the machining
direction) cuts into the material first.
|In Conventional , the rear of the advancing tool (in the machining direction) cuts into the material first.|
Specifies the maximum allowed distance between the theoretical and computed tool path.
Tool position ON guide
Specifies the position of the tool tip on the guiding element.
Specifies the engagement (A in trochoidal motion image) of the tool during trochoidal motion.
Specified the diameter of the trochoidal motion (B in trochoidal motion image), which corresponds to the width of the slot to machine.
Defines the maximum depth of cut in an axial strategy.
|Number of levels
Defines the number of levels to be machined in an axial strategy.
You can specify the following Geometry:
Guiding contours can be specified by:
The guiding contour can be restricted by means of Start and Stop relimiting elements. The tool can be positioned In, On or Out with respect to a relimiting element. You can select a point or a curve as relimiting element.
A fast way to specify relimiting points is to right-click the guiding contour area in the sensitive icon of the dialog box and set the Relimitation point detection contextual command. When you select a guiding contour, its extremities will be used as relimiting elements.
Note that a relimiting point can be created anywhere along the guiding contour by means of the Add relimiting point contextual command. Just right-click the relimiting element area in the sensitive icon of the dialog box and select any position along the guiding contour.
Relimiting point selection can be made easier depending on the selected screen view. For example, you can select the Normal View icon in the View toolbar and a suitable face. The screen view is then perpendicular to the selected face and it is then easier to define relimiting point locations on the guide when moving the cursor.
When relimiting elements are defined on a closed contour, the recommendation is to select the Close tool path option in order to respect the area to machine according to the Direction of cut (Climb Milling or Conventional) and the relimiting elements.
Only end mills can be used in Trochoid Milling.
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 check box is available for managing output of the SPINDL instruction in the generated NC data file. If the check box 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.
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. Corners can be angled or rounded.
For Trochoid Milling, feedrate reduction applies to inside corners. It does not apply for macros or default linking and return motions.
If a cornering is defined with a radius of 5mm and the Feedrate reduction in corners set to a lower radius value, the feedrate will not be reduced.
You can define transition paths in your machining operations by means of NC Macros. These transition paths are useful for providing approach, retract and linking motion in the tool path.
An Approach macro is used to approach the operation start point.
A Retract macro is used to retract from the operation end point.
A Linking macro may be used in several cases, for example:
A Return on Same Level macro is used in a multi-path operation to link two consecutive paths in a given level.
A Return between Levels macro is used in a multi-level machining operation to go to the next level.
A Return to Finish Pass macro is used in a machining operation to go to the finish pass.
A Clearance macro can be used in a machining operation to avoid a fixture, for example.
Note: When a collision is detected between the tool and the part or a check element, a clearance macro is applied automatically. If applying a clearance macro would also result in a collision, then a linking macro is applied. In this case, the top plane defined in the operation is used in the linking macro. The top plane element must be selected in order to apply an automatic linking macro without collision.