Return to PTConnector Home Page ToolsProductsDepartmentsResourceshelp
Home - Technical Support

go to www.ptc.com

Printer friendly version of this page

Email this page


   
Fax This 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.

mil672a

Figure 1


Procedure
  1. 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.
  2. 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.
  3. 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


  4. 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.

    mil672b2

    Figure 3


  5. 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.
  6. Select Play Cut to check the tool path. The tool path should resemble Figure 4.

    mil672c

    Figure 4


  7. 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.

    mil672d

    Figure 5


  8. 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.

    mil672e

    Figure 6


  9. 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.

    mil672f

    Figure 7


  10. 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.

P T C   I N T E R N A L   U S E   O N L Y
Intranet questions or comments? Email the Webmaster.
©1999 Parametric Technology Corporation