*Please lubricate holder before using.
We suggest ZENIPLEX II - Extreme Pressure Aluminum Complex Grease.
Drill
hole in workiece that is .005" to .015" larger than the smallest
diameter of broach to be used, and countersink this hole at 90° to slightly
larger than the largest dimension of the broach. Be sure to drill hose
deeper than the required depth of broach to allow for chip accumulation in
the hole.
When the broaching tool is
set up per one of the methods described below, advance it into the work as
the piece is rotating. The feed rate per revolution is calculated by
multiplying the drill diameter by .016 (EX: .250 dia x .016 = .004 IPR).
However, the feed rate must never be less than
.004 IPR or else a counterboring effect will occur.
*Oil
or a heavy water soluable coolant should be used to improve finish, extend
cutting tool life as well as tool holder life.
The
broaching cutting tool must have a 1-1/4 deg. back taper on all cutting
surfaces and should be dished on its face for freer cutting. It should
be made to the high side of the part tolerance to allow for maximum
resharpening for internal style broaches, and low side for external style.
Setting
the Holder for Center:
Nothing
is more important than having the cutter centered as close as possible to
the center of the workpiece. Improper center setting will cause uneven
hole configurations, oversize holes, spiralling, excessive cutter wear and
excessive holder wear.
Therefore,
it is essential that you observe the following instructions when setting up
broach cutters.
To
center cutter:
Clamp
shank of broach holder in a "V" block. Install
the broach cutter in the offset spindle hole and snug up the three (Pt. 5)
spindle screws.
While
rotating the offset spindle with the broach secured in it, adjust the three
(Pt. 5) spindle screws individually until the extreme end of the broach
indicates to within .001" concentricity. Lock broach securely in
place.
IMPORTANT!!
this step is essential since it is necessary to correct for the inherent
runout caused by the clearances between the mounting hole diameter and the
broach shank diameter and any eccentricities built into the holder spindle
and the broach itself.
Next:
To center the tool holder:
If
the machine shank mounting hole is in perfect alignment with the workholding
spindle, or if tool is being used on a CNC or vertical mill, proceed as
follows:
Loosen
the six (Pt. 8) body adjusting screws and the two (Pt. 7) clamp screws.
Loosen
the shank of the holder so that pressure is just snug enough to allow the
shank to rotate in the "V".
Rotate
the complete holder and indicate the extreme end of the broach as mounted in
the offset head assembly to within .001" TIR. (Do not rotate the
offset spindle.) Offset head is adjusted by tightening or loosening
the six (Pt. 8) body adjusting screws. When .001" TIR is
attained, lock offset head in place by tightening the two (Pt. 7) clamp
screws and the six (Pt. 8) body adjusting screws.
IMPORTANT:
This step is also essential to being certain that the extreme end face of
the broach is concentric with the shank of the broach holder itself.
If
the machine condition is such that the turret hole is not in line with the
spindle, the broach can be centered as follows:
Countersink
the hole at 45° to a diameter larger than the cross corners of the broach.
Loosen
the two clamp screws and six adjusting screws so that the body of tool is
free to move. Advance the tool holder into the workpiece, allowing the
broaching tool to center itself in the countersink of the workpiece.
While it is in this position, lock the body in place by tightening the six
adjusting screws and the clamp screws, being careful to not disturb the tool
alignment. If the tool does not cut the proper hole size, corrections
can be made by adjusting the six screws.
Hexagon
and square internal broaches as well as external broach blanks to fit these
holders are available as standard from stock at nominal prices.
These
same basic Instructions and principles for setting up, also hold true for
the Somma External Rotating Broach Tool. It is always a good idea to
turn 45 deg. chamfer on the workpiece to below the smallest diameter
of the broach even if it has to be turned off after broaching. Also,
broaching tool should not touch largest diameter of part being broached if
at all possible. I.D. of broach should have 1-1/4 deg. back
clearance. Grind 10 deg. to 15 deg. cutting angle on front face of
broach, preferably this should be faceted to coincide with shape of hole.
If you have a specific broaching problem you need
help on, please do not hesitate to contact
us. [Back to
Top]
