
|
|
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
- 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
- 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
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
- 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
- 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
- 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
- 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.
- 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
|