General Tips on Machining Kovar® Alloy
(Also known as ASTM F15, NILO® K, Pernifer® 2918, Rodar®, and Dilver® P1)
Characteristics I Coolant I Tooling I Turning I Drilling I Reaming I Tapping
Kovar ALLOY CHARACTERISTICS
Kovar Alloy is not hardenable by heat treatment.
Kovar can be made harder through cold working
only. The annealed hardness for Kovar Alloy
is generally in the range of RB 70/80, whereas
the 1¦4 H to 1¦2 H range for Kovar
between RB 80/96. In the annealed condition,
Kovar will be more difficult to machine because
it is soft and gummy. The tools tend to plow
the alloy instead of cutting into it and do
not easily form chips. Surface scale oxide
tightly adheres to and penetrates the surface
to a greater extent than stainless steels.
Machining is considerably improved by descaling
the material. If there were standard machinability
ratings applied for Kovar Alloy, Alloy AISI-B-1112
being measured as 100%, the percentage suggested
for Kovar would be (ASTM F15) 40%.
Kovar
ALLOY COOLANT
It is important to control heat buildup which
is the major cause of warpage. Suggested coolants
are Keycool 2000 or Prime Cut. Whatever lubricant
is used for machining, it should not contain
sulfur. Sulfur can effect the performance of
many sealed electronic parts.
Kovar
ALLOY TOOLING
T-15 Alloy, such as Vasco Supreme - manufactured
by Vanadium Alloys Company, M-3 Type 2 such
as Van Cut Type 2 - manufactured by Vanadium
Alloys Company. Congo-manufactured by Braeburn.
For machining with carbide tools, a K-6 manufactured
by Kennemetal, Firthite HA manufactured by
Firth Sterling, or #370 Carboloy could be used,
or a K2S manufactured by Kennemetal, or a Firthite
T-04 manufactured by Firth Sterling would be
satisfactory. One thing of prime importance
is that all feathered or wire edges should
be removed from the tools. They should be kept
in excellent condition by repeated inspection.
TURNING
Kovar ALLOY
If steel cutting tools are used, try a feed
of approximately .010" to .012" per
revolution and a speed as high as 35/FPM could
probably be attained. Some of the angles on
the cutting tools would be as follows:
End cutting edge angle - Approximately 7°
Nose radius - Approximately .005°
Side cutting edge angle - Approximately 15°
Back rake - Approximately 8°
Side rake - Approximately 8°
When cutting off, high-speed tools are better than carbide tools, and a feed of approximately .001" per revolution should be used. The cutting tools should have a front clearance of about 7° and a fairly big tip - larger than 25° would be helpful.
DRILLING
Kovar ALLOY
When drilling a 3/16" diameter hole, a
speed of about 40/FPM could possibly be used,
and the feed should be about .002" to
a .0025" per revolution, for a 1/2" hole,
approximately the same speed could be used
with a feed of about .0040" to .005" per
revolution. The drills should be as short as
possible, and it is desirable to make a thin
web at the point by conventional methods. By
conventional methods, we mean do not notch
or make a crank shaft grind. It is suggested
that heavy web type drills with nitrided or
electrolyzed surfaces be used. The hole, of
course, should be cleaned frequently in order
to remove the chips, which will gall, and also
for cooling. The drill should be ground to
an included point angle of 118° to 120°.
REAMING
Kovar ALLOY
Reaming speeds should be half the drill speed,
but the feed should be about three times the
drill speed. It is suggested that the margin
on the land should be about .005" to .010",
and that the chamfer should be .005" to
.010" and the chamfer angle about 30°.
The tools should be as short as possible and
have a slight face rake of about 5° to
8°.
TAPPING
Kovar ALLOY:
In tapping, a tap drill slightly larger than
the standard drill recommended for conventional
threads should be used, because the metal will
probably flow into the cut. It is suggested
that on automatic machines, a two or three
fluted tapping tool should be used. For taps
below 3/16", the two fluted would be best.
Grind the face hook angle to 8° to 10°,
and the tap should have a .003" to .005" chamfered
edge. If binding occurs in the
hole in tapping, the width of the land may
be too great and it is suggested that the
width of the heel be ground down. Again, it
is suggested that nitrided or electrolyzed
tools be used. Speed should be about 20/FPM.
Note: Applications specifically suggested for material described herein are made solely for the purpose of illustration to enable the reader to make his/her own evaluation. Guidelines are not intended as warranties, either expressed or implied, or fitness for these or other purposes. The data presented are typical of average values for all metal removal operations. They are not a guarantee of minimum or maximum values. Due to the distinguishing characteristics of each project, some metal/alloys may require adjustments (+/-) of speeds and/or feed which should be performed in small steps. Each job has to be developed for best production results with optimum tool life.