Thread Milling

Transcription

Thread Milling

COPYRIGHT © 2008, Seco Tools AB
1/71
Principles of Thread Milling
Threading Basics
Thread Milling Application Topics
Thread Milling verses Tapping
Thread Milling Advantages
Basic Application Techniques
2/71
Types of Threading
Types of manufactured threads:
• Thread turning
• Tapping (cutting)
• Roll tapping (cold forming)
• Thread milling
3/71
Quality of Threads Produced
• Tapping
75% thread depth (radial and
axial)
• Roll Tapping (cold forming)
- Limited applications
• Thread Turning, Thread
Milling
- 100% thread depth
- Strongest thread
4/71
Thread Milling
• Fast growing area in the cutting tool industry.
• Developed many years ago to produce high quality
threads, primarily in high temperature alloys, which
work hardened easily.
5/71
Thread Milling
Major
diameter
Minor
diameter
• External thread
• Internal thread
Major
diameter
Minor
diameter
90% Thread mill applications are internal
6/71
Thread Milling
Application Topics
•
•
•
•
•
•
•
•
•
Good workpiece clamping
Rigid machine and setup
Minimum cutter gauge length
Workpiece starting diameter
Most suitable cutter
Correct calculation of cutting data
Suitable cut division sequence
90o or 180o arc - in to cut
Controller CNC code compatibility
7/71
Thread Milling
Application Considerations
• CNC - Machining Center or Turning Center
• Helical Interpolation (very common)
Z
X
Y
8/71
Thread Milling
External RH thread
Down
milling
External LH thread
Down
milling
+Z
-Z
Internal RH thread
Up
milling
Internal LH thread
Down
milling
+Z
+Z
Through hole
Down
milling
Up
milling
-Z
-Z
Blind hole
9/71
Thread Milling Cutters
Threads are milled into the
workpiece using an endmill
style tool not a tap.
Types of thread mills:
Solid carbide
Single insert indexable
Mutli-insert indexable
10/71
Thread Milling Cutter Path
Top View
Begin 90° or 180° arc
interpolation into part.
Cutter
Rotation
11/71
Top View
Complete full rotation
around part. (helical
interpolation)
Cutter
Rotation
12/71
Thread Mill Cutter Path
Top View
interpolation out of
part.
Cutter
Rotation
13/71
Side View
Cutter rapids to axial depth
Cutter rapids to radial start position
90° or 180° arc into part.
(helical interpolation ½ pitch)
Start Position
14/71
Side View
Complete one full rotation around
hole moving in the “z” axis one
pitch.
(helical interpolation 1 pitch)
90° or 180° arc out of part.
(helical interpolation 1/2 pitch)
15/71
Side View
Cutter rapids to center of hole.
Cutter rapids to second axial
depth of cut.
Repeat previous cycle.
16/71
Cutter Path Detail
Move one pitch
P
17/71
Thread Milling vs. Tapping
Why thread mill when you can tap?
Tooling inventory (multiple tap sizes)
Multiple spindle starts and stops
Reduce horsepower and tool pressure
Tap breakage
Thread Starts
Chip Formation
Taper Thread
Hole Preparation
Half-hole situations
Helicoil threads
18/71
Why thread mill and not tap?
• Thread milling uses only one tool for through or blind holes.
• Tapping could use up to three taps.
Starting Tap
Plug Tap
Bottom Tap
19/71
Multiple Taps vs. One Insert
Left and Right Hand Threads
Right-hand
Left-hand
Two
Taps
vs. One mill
Thread Mill
One
thread
20/71
Two Threads - Same Pitch, Different Size
1/2” x 13
1” x 13
TwoOne
Taps vs.
One Thread
thread
millMill
21/71
Two Threads - Same size, Different Tolerances
1” x 13 - 3B
1” x 13 - 2B
Two
Taps thread
vs. One Thread
One
mill Mill
22/71
Tapping
Multiple Spindle Starts and Stops
1
Spindle M03,
Z down
2
3
Spindle M05,
STOP
Spindle M04,
Z up
23/71
Thread Milling
• Spindle M03, throughout thread milling operation
M03,
M05,
M04,
M05,
M03
24/71
Horse Power and Tool Pressure
Horsepower Consumption
•
Thread milling uses less
horsepower
Cutter
Path
Thread Mill
•
Creates less cutting pressure
• High Temperature Alloys
• Thin walled workpieces
• Hardened Steel
Cutter
Cutter
Rotation
Rotation
25/71
• Tap Breakage
- Requires additional EDM
machining process $$$
- Thread milling does not
26/71
Thread Starts-Tapping
Angular position can vary
27/71
Thread Starts - Thread Milling
Angular position always the same
28/71
Chip Formation - Tapping
Tapping produces long
continuous chips which tear
the workpiece material.
Re-cutting of chips may occur
resulting in tap chippage and
breakage.
Long continuous chips may
scar the thread surface.
mm
10
20
30
40
50
29/71
Chip Formation - Thread Milling
• Thread milling makes small, thin chips
• Superior thread form and finish
mm
10
20
30/71
Taper Threads
• Taper taps leave cutting-edge lines the whole thread
length
31/71
Taper Threads
X-section of taper thread
when tapped
32/71
Taper Threads – Thread Milling
Thread milling leaves no
marks - therefore no leaks!
Thread milling does not need
taper reaming like tapping
33/71
Drill Depth - Tap vs. Thread
Mill
Thread length 2 x D (20mm)
Tap
M10 x 1,5 ISO
Drilling
depth
27mm
Thread mill
M10 x 1,5 ISO
Drilling
depth
20mm
Drilling depth 100%
74%
Reduction
26%
34/71
34
Full Thread Depth - Tap vs.
Thread Mill
thread depth
thread depth
drilling depth
reduced
drilling depth
Thread Mill
Tap
lead
~3 x pitch
security = < 0,05mm!
security
~2 x pitch
35/71
Thread Depth
• Thread depth reduces as tap wears
• Controlled, consistent thread depth when thread milled
36/71
Half-Hole Situations
3 x Nr. 8 x 32 UNJC, Helicoil
37/71
Half-Hole Situations
Tap will deflect
It will break or spoil thread
Thread milling cuts one side of hole at any time
38/71
Helicoiled Threads
Special oversize
Tap needed $$$$
Easy with
standard
Thread Mill
39/71
Product Application
• Cutter path review
• Selecting Proper Cutter Diameter
• 90o or 180o arc - in to cut
• Radial engagement
• Calculating proper feed rate
• Selecting correct number of axial passes
• Selecting correct number of radial passes
40/71
Cutter Position Top View
Major dia
+
X Co-ord
Minor dia
Y Co-ord
41/71
Top View
interpolation into part.
Cutter
Rotation
42/71
Top View
Complete full rotation
around part. (helical
interpolation)
Cutter
Rotation
43/71
Top View
interpolation out of
part.
Cutter
Rotation
44/71
Selecting Proper Arc In Angle
Arc entry angle of 0°or straight line entry
•
never used
Cutter
Arc entry angle of 180° is used:
•
If cutter diameter is greater than thread
major diameter / 2
Major Thread
Diameter
Cutter
•
If cutter diameter is less than thread major
diameter / 2
45/71
0° Entry Arc Angle
Arc entry angle of 0° is never used:
•
Conventional milling path
•
Excessive chatter
cu
Excessive tool pressure
tte
r
r
o
t at
•
ion
cutter rotation
46/71
180° Entry Arc Angle
•
If cutter diameter is greater
than thread major diameter / 2
- gradual cutter engagement
ion
r
t te
u
c
cutter rotation
n
- superior finish
t
ta
ro
- no chatter
cutter
rotation
cutter
rotation
cutter
rotation
cutter rotation
cu
t
t
er
r
o
t
ati
o
- climb milling
47/71
90° Arc Angle Entry
Arc entry angle 90° is used:
•
If cutter diameter is less than
thread major diameter / 2
cutter rotation
cutter rotation
cutter rotation
cutter rotation
cutter rotation
cutter rotation
48/71
Typical Component Processing
CL
Thread
length
= 44mm
Insert
length
= 40mm
49/71
Current Practice
Axial depths of cut:
•
Cut 1 length = 40mm
•
Cut 2 length = 4mm
C
L
2nd cut
Results:
•
Unequal cuts
•
Unequal cutting forces
•
Two thread diameters
1st cut
50/71
Cutter Intersection Enlarged
A
B
A=B
At the end of the day,
it’s how gauge fits that
counts.
51/71
Preferred Method
Equal Depths of Cut
Axial depths of cut:
C
L
• Cut 1 length = 22mm
• Cut 2 length = 22mm
Results:
1st
cutcut
2nd
• Equal cuts
• Equal cutting forces
• One thread diameter
52/71
Preferred Method
Cutter Intersection Enlarged
B
A=B
At the end of the day,
the gauge fits.
A
53/71
Side View
Cutter rapids to axial depth
Cutter rapids to radial start position
90° or 180° arc into part.
(helical interpolation ½ pitch)
Start Position
54/71
Side View
Complete one full rotation around
hole moving in the “z” axis one
pitch.
(helical interpolation 1 pitch)
90° or 180° arc out of part.
(helical interpolation 1/2 pitch)
55/71
Side View
Cutter rapids to center of hole.
Cutter rapids to second axial
depth of cut.
Repeat previous cycle.
56/71
Radial Engagement Review
Stock removal depth = 0.500
Feed per tooth = 0.012
Feed rate = 252
Stock removal depth = 0.500
Feed per tooth = 0.009
Feed rate = 75
61/71
Axial Cut Divisions
• Axial depth of cut division considerations:
- Thread length
- Cutting edge length
- Set-up rigidity
- Machine rigidity
- Type of thread
1
- Type of material
Typically use the entire cutting edge length
If your unsure be conservative
3
5
62/71
Radial Cut Division
Radial with stock (material groups 1-4, 8-10, 15)

1 roughing cut

1 finish cut at .002” ae
Radial 2/3, 1/3 (material groups 5, 6, 11, 21, 22)

1 roughing cut at 2/3 of ae

1 finish cut at 1/3 of ae
Radial 1/3, 1/3, 1/3 (material group 7)

2 roughing cuts each 1/3 ae

1 finish cut 1/3 of ae
63/71
Holding System Comparison
Holder
Run-out
Rigidity
Shrink-fit
+++++
+++++
Always
Whistle notch
Seco sidelock
+++
+++++
Always
Hydraulic
+++++
+
Cylinder shank or
sleeve only
Sidelock
+
++
Yes, if not worn out
Milling Chuck
++
++
Yes, if used correctly
Recommended
64/71
Holding System Comparison
Holder
Run-out
Rigidity
ER Collet
++
+
Standard
Collet
+
+
Recommended
Yes, If used correctly
for solid carbide
No
65/71
Thread Milling Troubleshooting
Causes of failure in thread milling, in order of most
common occurrence:
• Rigidity
• CNC programming
• Cutting data
• Coolant
• Grade
• Work material
• Tool selection
66/71
Troubleshooting – Common Problem
First tooth of insert that is chipping is
common sign of rigidity problem
67/71
Thread Milling - Questions
Your company is a large laydown threading user and
threads a lot of internal components of different pitches.
You need to thread a component on a machine in
manufacturing to get production back up.
You see the only way to put thread on this external
application is to thread mill it.
Although you do not have the correct thread mill to do job.
What would you do?
68/71
Internal Threading Bar
Single point thread milling with a partial profile insert
69/71
Thread Mill Wizard
70/71
71/71

Thread Milling

Transcription

Similar documents

ZS10021_US Wandtafel Rev_B.indd - Sas