
|
|
Fax This Document (this feature currently
requires access to http://tortugas.ptc.com) | |
Suggested Technique for Defining a 5 Axis Trajectory Milling NC
Sequence Using a 2 Contour Cut Motion
This Suggested Technique explains how to create a 5 Axis Trajectory
machining NC sequence using 2 Contour. The first contour trajectory line
determines the direction the upper part of the tool will follow and the
second contour determines the direction that the lower end of the tool
will follow. Together, the direction and the tool angle can be determined
to generate the cut motion. In addition, synch points may be specified to
better control the time at which the top and the bottom of the tool follow
the trajectory. The model shown in Figure 1 is an example part requiring 5
Axis milling in the position shown.
Figure 1
Procedure
- To begin creation of the tool
path, the type of NC sequence must be chosen. Select Machining,
NC Sequence, New Sequence, Trajectory, 5
Axis, and Done.
- Select an appropriate tool,
coordinate system and retract plane using the Tool, Coord
Sys and Retract options respectively, if they have not been
previously established.
- NC sequence parameters must be
established before the tool path can be created. Critical parameters are
shown in Figure 2.
CUT_FEED |
15 |
TOLERANCE |
.001 |
SPINDLE_SPEED |
500 |
CLEAR_DISTANCE |
.100 |
|
Figure 2
- When defining an Automatic Cut in
release 2000i2 of Pro/ENGINEER, the Customize dialog box appears. For
more information on the new Customize dialog box, please see the Suggested
Technique for Demonstrating the New User Interface in the Customize
Environment. For this example, select Insert, Two
Contour, and Done to accept the defaults. From the TRAJ OPT
menu choose Select, and Tangent Chain. Pick the top inside
edge of the part as shown in Figure 3 and then select Done. To define
Contour 2 pick Select, Tangent Chain, and select the
bottom inside edge as shown in Figure 3.
Figure 3
- The next step is to define a
surface for the tool tip to follow. In this example, select the bottom
surface of the part, Done Sel, and Done/Return from the
HEIGHT menu. Flip the red arrow in the direction the tool should
travel and select Okay. Define the tool offset by selecting
either None, Left, or Right, and then select
Done.
- Select Play Cut to check
the tool path. The tool path should resemble Figure 4.
Figure 4
- Notice the angle of the tool in
the corners as seen in Figure 5. Move the tool around the tool path be
selecting either Next or Prev. At the position in Figure
5, the tool axis needs to be constrained so that it is parallel with the
radius tangency. This can be accomplished by adding Synch points.
Figure 5
- Create the Synch points by
selecting Define Cut, checkmark Synch, and Done.
Pick the locations shown in Figure 6. When finished, select Done
Select and Done/Return.
Figure 6
- Replay the tool path be selecting
Play Cut and move the tool around the tool by selecting
Next and Prev. Notice the change in Figure 7 v.s. Figure
5.
Figure 7
- To complete the creation of the
cut motion, select Done Cut and the Follow Cut dialog box should
appear. For this example, select Default and Okay. From
the Customize dialog box select OK. The tool path can be viewed
again by selecting Play Path and Done.
|