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 Creating a Profile Milling Sequence with an Approach and Exit defined.


This Suggested Technique describes how to create a profile milling toolpath with LEAD_IN and LEAD_OUT functionality along with the Approach and Exit axis for the tool to approach and exit which will be defined in the Build Cut level in a 3-axis profile milling sequence.
Procedure
  1. To begin creation of a Profile Milling NC sequence for the model shown in Figure 1, the type of NC sequence must be chosen. Select Machining NC Sequence, New Sequence, Profile, Done. This presents the NC SEQUENCE and SEQ SETUP menu which contain all the options necessary to define the NC sequence.

    Figure 1


  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 CUT_FEED, STEP_DEPTH, SPINDLE SPEED and CLEAR_DIST. To set the parameters LEAD_IN, LEAD_OUT and LEAD_RADIUS, in the Param Tree select Advanced and set LEAD_IN and LEAD_OUT to YES and specify a value for LEAD_RADIUS as shown in Figure 2,  The other values should be appropriate to your machine and material, but must be entered.

    CUT_FEED 50
    STEP_DEPTH 0.75
    SPINDLE_SPEED 500
    CLEAR_DIST 0.2
    LEAD_IN YES
    LEAD_OUT YES
    LEAD_RADIUS 0.5

    Figure 2


  4. Next the surface to be machined must be defined. For this example, select Model  and Done from the SURF PICK menu and select the surfaces shown in Figure 3. Once the surfaces have been selected, select Done Sel, Done and Done/Return.

    Figure 3


  5. To define the Approach and Exit axis, select Seq Setup from NC SEQUENCE menu, check Build Cut, Done. Select Approach from NC BUILD CUT menu and keep the default menu picks Point, Each Slice and select Done from PATH DEFN menu. If the Axis is already available use the default menu pick Select to select the axis. In this example, an axis is created in the Manufacturing Model so select the menu pick Create to create the axis. Then from DATUM AXIS menu select Pnt Norm Pln and select the top surface of the model for the normal plane as shown in Figure 4.

    Figure 4


  6. Select Create Point from GEN PNT SEL menu and pick Offset Surface from DATUM POINT menu. Select the surface from the model for the tool to approach and the respective edges for the dimension to fix the point as shown in Figure 5. In this example, the dimensions from the edges is given as zero and the offset distance is 4 as shown in the arrow direction. The point will get created and pick Done from DTM PNT MODE menu and Done from GEN PNT SEL menu then the axis will get created as shown in Figure 6.

    Figure 5

    Figure 6


  7. To define the Exit Axis, select Exit from NC BUILD CUT MENU  and select Done from PATH DEFN menu. Keep the default pick Select and pick the same axis created for Approach as the Exit axis and select Done Return from NC BUILD CUT MENU.
  8. To view the tool path, choose Play path and Screen Play from the PLAY PATH menu. Using the PLAY PATH dialog box, select the Play Forward button to view the tool path. The resulting tool path for this example is shown below in Figure 7.

    Figure 7



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