-
Activate the Manufacturing Program and click
Facing
in the
Prismatic Machining action bar.
A Facing entity is added to the
Manufacturing Program.
The Facing dialog box appears directly at the Geometry tab . This tab
includes a sensitive icon to help you specify the geometry.
The part bottom and flanks in the icon are colored red indicating that this
geometry is required for defining the operation. All other geometry is
optional.
- Still in the Geometry tab, select the required geometry.
See Selecting Geometry - Right-click the red bottom in the
icon and select Contour Detection in the context menu.
- Click the red bottom then select the
underside of the part in the 3DEXPERIENCE platform.
The Contour Detection option automatically deduces the part boundary.
This is indicated by the highlighted drive elements. The bottom and flanks of the icon are
now colored green indicating that this geometry is now
defined. - Select the Strategy tab
.
- Choose the desired Tool path style: Inward
helical, Back and forth, or One
way.
- Set the machining criteria such as Machining
tolerance, the radial strategy (see below), the axial strategy (number of levels= 1, for example), the finishing parameters, the HSM parameters (for
Inward helical Tool path style only), and User Parameters.
Tool path style: Back and forth
Mode: Maximum distance Distance between paths: 40mm End of path: Out Overhand: 50 Tool side approach clearance: 2.5mm
- Go to the Tool tab to select a Face Mill tool.
See Assigning a Tool Element to a Machining Operation - Select the Feeds and Speeds
tab to specify the feedrates
and spindle speeds for the operation.
- Select the Macros tab
to specify a return in a level macro, which is necessary
for the One Way mode.
See Defining Macros on Milling Operations - In the Macro Management frame,
right-click the Return in a
Level Retract line and select
Activate.
- In the Current Macro Toolbox
frame, select the Axial
mode. A sensitive icon representing
this retract motion is displayed.
- Double-click the distance parameter
in the sensitive icon and
enter the desired value in
the pop-up dialog box.
- Select the Return in a
Level Approach line, then repeat
the procedure to specify the approach
motion.
-
Click Display or
Simulate to check the validity of the operation.
See Simulating the Tool Path.
- The tool path is computed.
- A progress indicator is displayed.
- You can cancel the tool path computation at any moment before 100%
completion.
- Click OK to create the
operation.
-
If you want to define a different start
point, click the start point symbol
in the sensitive icon in the Geometry
tab then select a point.
Note:
The exact position of operation
start point may be different from your
selected point. The program choose
the nearest point from a number of possible
start positions.
|