The Turning Page “the Turning Revolution”

Broaching On A CNC Lathe

One operation seen on many turned parts today is broaching. Traditionally
broaching has been regarded as a secondary operation that was typically performed
on a broaching machine with special broaching tools. Depending on the industry,
much of this type of broaching is still being done in this manner. For instance, in the
automotive sector, almost all broaching is done by large expensive automatic
broaching machines with specially designed broaching tools that can produce the
broaching at very high speed and short cycles.
Of course the fact that they are doing over a million parts per year has much to do
with their method of manufacturing the parts. But today, even in the automotive
sector, the need for JIS and reduced inventory, can justify doing parts complete on a
single piece of equipment such as the multi-axis turn/mill center. With this
equipment, a new job can be easily modified and reconfigured for revision and
design changes. This is where flexibility wins out over speed.

Types Of Broaching.

There are a few different types of broaching that can be performed on the
CNC lathe.
#1. Single slot broaching on the inside or outside diameter of a part.
#2. Multiple shapes such as hexagons or squares.
#3. Timed broaching or broached slots that require an angular position to
another feature on the part.
#4. Free position broaching that does not require an angular position to
another feature n the part.
#5. Rotary Broaching
#6. Reciprocating Broaching
The type of broaching you need to do, will determine your tooling choice and
method.

ROTARY BROACHING

One of the easiest and fastest ways to produce a broached feature is Rotary
or Wobble broaching. Rotary broaching has been around for years in the screw
machine industry and is very effective, inexpensive and fast. It is used widely in the
manufacturing of plumbing parts such as valves and fittings and in the aerospace
and medical industries. When your parts require a single broached polygon that is
not related to another angular orientation or feature on the part such as a milled
flat or drilled hole, this is often a first choice.

A leading US company in the manufacture of Rotary broaching tools and
accessories is Slater Tool Company from Clinton Township, Michigan. They can be
found on the web at www.slatertools.com where they list a full complement of rotary
tool holders, tool bits, and detailed application documentation.

A simple example of this type of rotary broaching is the producing of an I.D.
hex on the end of a part. Let’s say it is a 5/8 hex in 12L14 steel. First thing is to
determine the max hole to drill, and then the size chamfer needed to make a good
acceptable hex. This can be determined by multiplying the hex size by 1.035 to
determine the largest pilot hole to be drilled.
Hex size .625 x 1.035 = .646 Pilot Drill = .625 to .646 diameter.

To determine an acceptable chamfering size, multiply the hex size by 1.1547
Hex size .625 x 1.1547 = .721

Next is necessary to determine the feed for the type of material and broaching tool.
For the 12L14 steel, according to Slater Tool’s web site, we should broach this at
1200 RPM with a feed of .006 i.p.r.

Here is a simple program example using the rotary broach tool programmed for a
Eurotech 735SLY.
O2007(ROTARY BROACH EX)
G0G40G80
N1G54T0101M64(.633 DRILL)
G0G99G97S3620X0Z.1M3M8
M58(LOAD MONITOR ON)
G1Z-.75F.016
M59(LOAD MONITOR OFF)
G0Z1.
M1
N2G54T0202M64(3.4 90 DEG. SPOT)
G0G99G97S635X0Z.1M3M8
G1Z-.3F.03
Z-.3605F.003
G4P100(DWELL)
G0Z3.
M1
N3G54T0303M64(5/8 ROTARY BROACH)
G0G99G97S1200X0Z.1M3M8
G1Z-.65F.006
G0Z.1
G28U0M5
M30
TOTAL PER TOOL
DRILL = 4.5 SEC. CHAMFER = 5 SEC. BROACH = 8.5 SEC.
TOTAL CYCLE TIME = 18 SEC.

NOTES AND TIPS FOR ROTARY BROACHING:
Special attention should be made to how well the tool is aligned in accordance with
the Rotary broach supplier. Miss-aligned tools will result in poor tool life and
surface finish.

This application is not suited for parts where other features such as milled flats,
slots or drilled hole patterns are related to the fixed position of the polygon
produced by the Rotary broach.
Coolants or oils are required to clear chips and reduce friction for better tool life
and surface finish.

SINGLE SLOT BROACHING

When single or multiple broach slots are required they can be done on the
CNC lathe using a single broaching tool either carbide or HSS. This type of
broaching requires the CNC to have C axis for spindle positioning and a spindle
brake to hold the spindle steady and firm while broaching. Multiple passes are
required and can be programmed easiest by using sub programming and/or macro
programming. Next we will examine both styles of programming to help determine
what best suits the programmer and the part.

Note that most broached slots should have a groove broach relief or go all the
way through the part. It is not recommended to use this broaching technique into a
blind hole or one without a groove relief. Another important item is to retract the
broaching tool completely from the broached slot before feeding or rapid traversing
back to the Z start position.

EXAMPLE: .250 broached slot through .500 deep from face.

Programmed for a Eurotech 735SLY.
Sub Program.
O1444(SUB FOR .25 WIDE BROACHED SLOT)
G0X[#103](#103= .002 RADIAL DEPTH OF A PASS)
G4P100(SMALL DWELL)
G1G98Z-.5F200.(FEED BACK .5 AT 200 INCH/MIN.)
G0X.6(CLEAR THE HOLE DIAMETER)
Z.2(RETURN TO STARTING Z)
#103=[#103+#102](UPDATE #103 TO EQUAL NEXT X VALUE FOR A PASS)
M99(REWIND)

Main Program
O1234(MAIN)
XXXX
XXXX
XXXX
(SET COMMON VARIABLES FOR BROACHING)
#101=.624(BORE DIA. LESS .001 TO MAKE EVEN # OF PASSES)
#102=.004(X DEPTH OF A SINGLE PASS)
#103=#101+#102(BORE .624 + .004 = X VALUE FOR A PASS)
N5G54T0505M64M5(.250 wide broach)
M10(C AXIS ON)
G0X.624Z.2C0.M8
M70(SPINDLE BRAKE ON)
M98P331444(CALLS SUB PROGRAM 1444 TO REPEAT 33 TIMES)
M71(BRAKE OFF)
M11(C AXIS OFF)
G0X4.Z2.
M1
XXXXXXX
XXXXXXX
XXXXXXX
M30
NOTES AND TIPS FOR SINGLE BROACHING:
The 1st. pass is X.628 (.624+.004)
The 2nd pass is X.632 (.628+.004)
Etc.
Etc.
The 33rd pass is X.756 (.752+.004)
X.624 Start from X.756 End = .132
.132/.004=33 passes
Often a G4 (Dwell) or a greater Z start value is used before the beginning of each
pass to minimize any taper caused by Servo Lag.
Macro Variables #100 – #199 are not held in Macro Offsets when the machine is
powered off. If you want the macro values retained in the offsets when the machine
is powered off, use #500-#999
Estimated Time to complete this single broach = 12 sec.

If you need to make more of the same broach at different angular positions, your
main program would look like this……
O1234(MAIN)
XXXX
XXXX
XXXX
(SET COMMON VARIABLES FOR BROACHING)
#101=.624(BORE DIA. LESS .001 TO MAKE EVEN # OF PASSES)
#102=.004(X DEPTH OF A SINGLE PASS)
#103=#101+#102(BORE .624 + .004 = X VALUE FOR A PASS)
N5G54T0505M64M5(.250 wide broach)
M10(C AXIS ON)
G0X.624Z.2C0.M8(INDEX TO 0 DEGREES)
M70(SPINDLE BRAKE ON)
M98P331444(CALLS SUB PROGRAM 1444 TO REPEAT 33 TIMES)
M71(BRAKE OFF)
G0C90.(INDEX T0 90 DEGREES)
M70(BRAKE ON)
M98P331444(CALLS SUB PROGRAM 1444 TO REPEAT 33 TIMES)
M71(BRAKE OFF)
G0C180.(INDEX TO 180 DEGREES)
M70(SPINDLE BRAKE ON)
M98P331444(CALLS SUB PROGRAM 1444 TO REPEAT 33 TIMES)
M71(BRAKE OFF)
G0C270.(INDEX T0 270 DEGREES)
M70(BRAKE ON)
M98P331444(CALLS SUB PROGRAM 1444 TO REPEAT 33 TIMES)
M71(BRAKE OFF)
M11(C AXIS OFF)
G0X4.Z2.
M1
XXXX
XXXX
XXXX
M30

BROACHING MACRO
Another alternative is to create a Macro program for your broaching requirements.
The advantage to creating a complete Macro program is you can use the one basic format
for most of your broaching needs. Below is one example of a broach Macro program used
for the same broached part from our previous sample.
Macro Variables –
#100 = Diameter of Bore to be Broached
#101 = End of Broach Slot Diameter
#102 = Broach Feed Rate
#103 = Starting Z
#104 = Ending Z
#105 = Amount of Dwell Before Cut
#106 = Depth of Cut Per Pass
#107 = Diameter to Clear Broach Slot
PROGRAM – 735SLY
N8 G54 T0808 M64 M5 (.250 WIDE BROACH)
#100=.624
#101=.756
#102= .200
#103= .200
#104= -.500
#105= .1
#106=.004
#107=.600
M10 (C AXIS ON)
G0 X#107 Z.5 C0 M8
M70 (BRAKE ON)
G0 Z=#103 (MOVE TO Z START)
WHILE[#101GT#100]DO1
G1G98X[#100+#106]F#102 (X VALUE FOR A PASS)
G4U#105 (DWELL)
9
Z#104 (ENDING Z)
G0 X#107 (CLEAR BROACH SLOT)
Z#103 (RETURN TO Z START)
#100=[#100+#106]
END1
#100=.624 (RESET VALUE)
G0Z.5 M71 (BRAKE OFF)
M11(C AXIS OFF)
X4. Z2.
M1(OPTIONAL STOP)
NOTES AND TIPS FOR BROACHING MACRO:
The WHILE and DO statements for this Macro program are recommended over the
use of a IF and GOTO statement. An IF statement requires a GOTO that searches
for the specific BLOCK number directed by the GOTO. Because of this block
search, the processing time is greater and would add to your broaching cycle time.
Example:
Instead of the WHILE and DO, we could have used the IF and GOTO.
IF[#101GT#100]GOTO555
This statement would send the machine to BLOCK N555 and repeat again until
#101 is equal to or less than #100.
The Macro program would need to be re-written with the IF statement located at
the completion of 1 broach pass.

RECIPRICATING BROACHING
High speed reciprocating broaching is becoming more and more popular and
is the first choice for anyone doing a large amount of production broaching on their
CNC equipment. Today’s high speed broaching units are mounted onto the turret
and use the live tool drive system to send the tool forward and back at faster stroke
speeds than can be achieved by the machine’s rapid traversing.
The primary benefits to this type of broaching are ….
?? Speed (reduced cycle times)
?? Increased Tool Life
?? Less machine wear or Slide Working

At stroke speeds of up to 700 strokes per minute, these units can produce
broached slots in a third of the normal single stroke fixed broach with better tool
life. Since the live tool drive system is driving the tool to reciprocate, the machine
slide stays fixed, providing added rigidity and less wear and tear on the machine as
a whole.

This entry was posted in Business. Bookmark the permalink.