Transcript Cost Drivers - H&S Manufacturing Co.

H&S Manufacturing Co.
Correlations between
DESIGN & COST
in precision metal
Expertise
$ Cost Drivers $
Innovation
Experience
contract manufacturing
H&S Manufacturing Co.
contract manufacturing
Agenda
Introduction
Documentation
Design
Tolerance
Cosmetics
Closing
This very much an interactive
discussion. The floor will remain open
for questions and open discussion
regarding any topic.
Introduction
•
•
This presentation was
designed to share knowledge
and stimulate discussion on
various design
characteristics and how they
affect cost of fabricated
precision sheet metal and
machined parts. We will
cover fabricated parts
manufactured by cutting
(punch/laser), forming,
milling, finishes, and
cosmetics. In some cases we
will distinguish between
‘sheet metal’ and ‘machined’
parts and note those
differences.
Sheet metal typically refers to sheet materials that
range in thickness from .020” (.5mm) to
.250”(6.4mm). Thinner materials are often called
‘shims” while thicker material is often referred to as
“plate” or “ingot”. At H&S we typically work with
thicknesses from .020”(.5mm) to .125” (3.2mm).
Again these are typical and may vary depending on
the requirement. The sheets are then cut and formed
in various methods to produce the desired part.
Introduction (cont.)
• The precision aspect of this industry has to do
with the dimensional accuracy of the finished
parts. For sheet metal the sheet thickness of the
raw material is typically within 5% of nominal.
Sheet metal equipment typically can hold
dimensions to within .005”(0.13mm), and bends
within 1/2 degree. Please note this is typical
repeatability for brand new equipment. In
machining the raw material tolerances are
typically of no concern. In most cases with the
exception of machining castings and extrusions
all surfaces are cut therefore tolerances of the
raw material has no bearing on the finished
parts dimension, only how the finished
dimension is achieved.
Introduction (cont.)
• Machining typically refers to the removal of
material with a cutter of various types to
produce the desired part. The material shapes
typically used are plate, bar, round, tube, pipe,
or extruded material. At H&S we focus on
milling which involves feeding the raw material
or part past a rotating cutter with cutting edges
on its sides, end or both. In contrast, turning
along with milling the most common machining
methods, rotates the raw material or part
around its axis and a cutting tool is feed parallel
to the axis to create a cylinder or at right angles
to the axis to create a face.
Documentation
Clear legible documentation is imperative.
Remember in most manufacturing environments
the large majority of ‘users’ of prints are not
formally trained or educated on print
interpretation. Obviously skill levels vary and
while most experienced sheet metal mechanics
and machinist are very proficient at reading
prints not all operators and laborers are. In fact
many have less than a high school education.
Almost all are trained ‘on the job’, and many
have languages other than English as their
primary language. This is common in
manufacturing plants all over the world. The
point being if the print is prepared in such away
as to require a senior level, higher wage, more
experienced person to understand its meaning
the manufacturer must allow for that financially.
The ease at which the information can be
deciphered can reflect dramatically on the
quality and efficiency of the manufacturing
processes used to produce the part. Below are a
few items that should be considered when
preparing a print. In short understand the target
audience or user of the documentation.
Documentation (cont.)
Revision control: A revision level on each print
ensures that the customer and manufacturer are
‘on the same page’. Revision levels should be
changed regardless of how minor the change is.
The effort will reduce brain damage in the long
term.
Title blocks: A title block should include the part
description, part number, revision. Items that
may be in a title block are cad file name,
engineering approvals, tolerances, dates.
Documentation (cont.)
Geometric Dimensioning &
Tolerance: GDT can be a
good thing, if it is used
properly and drafted
correctly. It is an excellent
method of showing
important relationships
between features, bends,
edges, etc… It helps
inspection by detailing the
critical dimensions necessary for functionality. There are
cautions and considerations that should be taken when
using this dimensioning scheme. GDT typically requires
greater effort from the designer but can yield much more
cost effective designs with more efficiently producible
parts than an over toleranced part. Secondly GDT will
typically require higher skill level employees to produce
and inspect and can require the use of more sophisticated
inspection equipment than standard toleranced parts.
However, if there is a requirement for tighter tolerances
on certain features using GDT can focus those additional
efforts to the specific dimensions necessary rather than
wasting those efforts on all dimensions if the part is over
toleranced.
Documentation (cont.)
Location of zero datum: When dimensioning a
drawing it is recommended to keep in mind
typical inspection methods used in
Manufacturing. For example most sheet metal
will be measured using hand held calipers
during the manufacturing process. The location
of the zero datum can result in more calculations
necessary to measure the part. The more
calculations, the less efficient the process and the
chance of error will increase. While hand held
calipers are used to measure some dimensions on
machined parts most are measured using a
height gauge on a flat inspection table. This is a
slower method but necessary for tighter
tolerance machined parts. This does allow for
easier location of the zero datum to measure
dimensions than with hand calipers.
Design
Below are general comments concerning
specific design features of both sheet
metal and machined parts.
Holes or Features/formed and flat
Flange Size
Bend Radius
Bend Relief
Standardization
Design (cont.)
Holes or features/formed and flat
One question that comes up regularly is: How
close to a bend can a hole be located? First a
hole or cut out of any shape can be located right
in the middle of a bend. However that shape will
be distorted during the forming/bending process.
Formed features can not be located such
generally speaking or they would be flattened or
misshaped during the forming/bending process.
Normal bending procedures are enabled when
the edge of a hole or feature is at least two
material thicknesses away from the start of the
bend. This rule can hold for most formed
features however depending on the direction of
the form and the die combinations necessary to
form the part relief modifications may be
necessary to the brake tooling to clear the
formed feature. Unformed features and holes
closer than two material thicknesses typically
require the use of backup material which adds
additional manufacturing time and could still
result in disfigured holes or features and process
variations.
Design (cont.)
Flange size
Another common question concerns flange sizes.
In material thicknesses ranging from
.020”(.5mm) to .125” (3.2mm) we typically deal
with a good general rule for inside minimum
flange length is three times the material
thickness plus the inside bend radius. Coining
with thinner materials can yield a smaller radius
but requires additional considerations such as
reduced material strength (aircraft industry
forbids coining), more pronounced brake marks,
etc…
Bend Radius
A minimum bend radius is another hot topic.
Another general rule of thumb for a minimum
bend radius is the inner radius should be at least
one material thickness. Thicker material and
sometimes more brittle material require larger
bend radius to avoid the material cracking.
Design (cont.)
Bend Relief
Bend relief’s are cutouts or holes to prevent
tearing or cracking of material when the part is
formed. Forming without tearing or cracking
the material will improve the accuracy and
consistency of the part during production.
Relief’s are typically specified as shop option
and are not dimensioned or marked as ‘no
inspection’. Minimum bend relief’s are one times
the material thickness plus the inside bend
radius.
Design (cont.)
Standardization (Boring)
A major cost consideration in metal design
should be standardization. If a design or group
of parts is ‘boring’ because the same design
feature is called out over and over it is likely the
cost of the products have been reduced.
Conversely if the design is constantly pushing
everything to the limit and each feature is
unique costs have been inflated. Some examples
might be to use the same piece of hardware
through out a design, the more we buy the less
we pay, the less we pay the lower your costs.
Understand when selecting items from
catalogues or websites what items are standard,
off the shelf, and which ones are ‘special’ or
‘custom’. Special and custom are always buzz
words for more cost and they (the seller) want
you to use them because they make more money
on them. Use the same radius call out on a
machined part, less set up time, less tool
changes, more efficient run time, less cost.
Remember increased buying power (more of one
thing than a few of many), reduced set ups (on
size tool vs. many different), less inspection time,
better quality, can all be positive, cost saving by
products of more consistent designs.
Design (cont.)
Designers know their designs better
than anyone else. Most manufacturers
or vendors see many designs or prints
every day. So designers can play a vital
role in communicating consistent or
similar designs or pointing out
consistent or similar features across a
family of designs.
Tolerance +/Back in the day, "build-to-order" sheet metal
tolerances were +/-.06" (1.5mm), primarily due
to the accuracy of the equipment. Today, normal
production tolerances are around 15% of that.
Tolerance ranges should be "reasonable" or
"practical" for the application.
The most significant improvement has been in
the machinery. Some modern high speed
equipment can position within .004" (.10mm)
and repeat within .002" (.05mm). This
repeatability is for new equipment. Materials
and methods continue to play a role in the limits
of precision, however. They greatly influence
practical considerations for tolerances between
holes (hole to hole), between bends (bend to
bend), and so forth. If tighter tolerances are
needed, they can be achieved with dedicated
tooling and special processing. However, it is a
mistake to simply dimension all mating parts
expecting +/-.005” (.127mm) accuracy. Any
‘over’ tolerance forces additional labor in
sorting and inspection and can result in
excessive scrap. Therefore the end result of
tolerances that are too tight is higher costs and
lower productivity.
Tolerance (cont.)
Hole Sizes
One method to produce a hole is by mechanically punching a tool
through sheet metal into a die tool to rip out a slug and form a
hole in the sheet metal. The size and shape of the punch and die
tooling determine the size and shape of the hole. The minimum
size hole or feature produced this way must be at least 1 ½ the
material thickness. The die tool must be slightly larger than the
punch to minimize tooling wear and to reduce the pressure
required too punch the feature. This difference in the punch and
die tool size is called ‘clearance’ or ‘die clearance’. The die
clearance is generally about 10% of the material thickness. For
example, if the material is .100” thick aluminum and the punch
diameter is 1.000", the die diameter would be 1.010". The size of
the hole on the punch side will be the same size as the punch tool.
The size of the hole on the die side will be the same size as the die
tool. This is referred to as ‘blow out’. Except for tooling wear,
there is very little variation from one hole to the next. Most
fabricators look to the engineers and draftsmen to give a
tolerance range that allows the use of existing tooling. When that
is not possible, a capital investment in new tooling is required.
Generally speaking, +/-.003" (.08mm) is a reasonable hole size
tolerance for punching holes. Keep in mind, however, that we are
measuring what will pass through the hole, not the "rim sizes" of
the hole.
Tolerance (cont.)
If required, tighter tolerances can be held on holes
produced by machining a hole using mill. This
method of production can also be used if ‘blow out’
described above is unacceptable. For machined parts
this is the preferred method. However, for sheet
metal parts this method is less efficient and adds cost
to the part. Standard hole size tolerances for
machining applications are +/-.003”(.08mm). With
many variables that should be considered machined
holes can be as tight as +/-.0005 (.013mm). However
considerations must be given to material, hole depth,
hole location (length of tool needed), thru or blind
hole, drilled or generated, etc…
Tolerance (cont.)
Hole to Hole (within the same surface)
The accuracy of the distance from one hole to another
hole is primarily dependent upon the machinery.
Most modern equipment will hold better than +/.005" (.13mm) However, each feature punched
introduces stress into the sheet metal. If the part has
many closely spaced holes or features such as
perforated patterns or formed features such as
counter sinks or lances, the result can cause the sheet
to warp or distort which can cause unwanted
variations between holes and features. A standard
tolerance for hole to hole would be +/-.010" (.25mm)
especially in areas where a large percentage of
material is being removed. Use tighter tolerances, as
low as +/-.005 (.12mm), only when absolutely
necessary.
In machining the amount of material being removed
is also a large contributing factor in hole to hole
tolerances. As heat builds in the part and cutting
instrument material moves and causes variation.
However in the machining processes this is very
controllable and allows for much tighter tolerances to
be achieved. Keep in mind however the tighter the
tolerance the more labor again for sorting and
inspection. Also less efficient production results in
reducing feeds and speeds of the machinery to achieve
the tighter tolerance which adds cost to the part.
Standard hole to hole tolerances for machining
applications are +/-.005”(.12mm).
Tolerance (cont.)
Hole to Edge (within the same surface)
In most modern sheet metal fabrication the profile (or
edges) of the part are generally punched or laser cut
just like any hole. Therefore the same considerations
for hole to hole apply. When features are produced by
punching very near to an edge (less than 1X the
material thickness) the edge can be pushed out by the
stress of punching the metal or in the case of cut outs
parallel to an edge the remaining web can roll or
twist. This edge migration introduces variables in the
accuracy of the location of a hole or feature to the
edge. A standard tolerance for hole to edge would be
+/-.010" (.25mm) especially in areas where holes or
features are less than the minimum distance
recommended from the edge. Use tighter tolerances,
as low as +/-.005 (.12mm), only when absolutely
necessary. Additional considerations should be given
to the use of the hole or feature. If hardware is to be
inserted most hardware manufactures publish a
minimum edge distance to insure no distortion upon
hardware insertion.
Similar considerations for machined parts hole to hole
tolerance should dictate hole to edge tolerance.
Standard hole to hole tolerances for machining
applications are +/-.005”(.12mm).
Tolerance (cont.)
Hole to Bend (dimensions across one bend)
Several factors have been introduced leading up to
this stage in the sheet metal fabrication process.
Features and parts have been punched on a CNC
turret press and/or cut using a laser, line sanded or
tumbled to remove burrs, and now is being formed on
a press brake. The deburring process can remove as
much as .003” when cosmetic appearance is a priority.
Precision press brakes will position and repeat within
the +/- .002” range. Skilled brake operators are able
to load the parts for forming consistently from bend
to bend. Nevertheless, consideration must be given to
the natural variation in material thickness (5% of
nominal thickness), the variation or tolerance from
the turret press or laser cutting, the effects of cosmetic
sanding, and the variation introduced by the press
brake plus variations in future processes like plating
or painting. A tolerance of +/-.015” hole to bend is
functionally reasonable for most applications. Resort
to +/-.010” only when absolutely necessary. Use
tighter tolerances, as low as +/-.010 (.25mm), only
when absolutely necessary.
Tolerance (cont.)
Bend to Bend (dimensions across multiple bends)
All of the considerations of hole to bend apply,
compounded by the fact that multiple material
surfaces and thicknesses are involved. Those
variations will be multiplied by factors of at least
two and sometimes many more depending on the
number of bends across the dimension. Standard
tolerance should allow +/-.020" (.50mm) bend to
bend. Use tighter tolerances, as low as +/-.010
(.25mm), only when absolutely necessary.
Tolerance (cont.)
Gauge Tolerance
Gauge tolerance is the tolerance of the devices
used to measure or inspect the products being
manufactured and must be considered when
applying tolerance. As stated earlier most sheet
metal with standard tolerance is inspected on
the manufacturing floor using hand held
calipers. A good, calibrated set of calipers will
have a tolerance of +/-.001 (.025mm) were as a
well maintained top of the line height gauge will
have a tolerance of +/-.0005 (.13mm) and is used
more inspecting machined parts.
Tolerance (cont.)
Tolerance Summary
Sheet Metal
Were as brand new machinery and proper
tooling will repeat within .004" (.10mm), it is
a mistake to simply dimension all mating
parts expecting +/-.005" (.13mm) accuracy.
Such over kill forces additional labor in
sorting and inspection, excess scrap, and less
manufacturing efficiency. The result of
tolerances that are too tight is simply higher
cost and lower productivity. Parts having
correct tolerance still have excellent fit and
function, with the added benefit of efficiency.
Tolerance (cont.)
Tolerance Summary (cont.)
Machining
When dimensioning machined parts tighter
tolerances are typical. One should however still
consider the cost impact of the tolerances
designed into the part and remember the effect
tolerance overkill can have on the efficiency and
productivity of the manufacturing process.
Summary
For both cost and manufacturing efficiency one
must consider the sum of the variables involved
affecting tolerance. From machine capabilities,
material limitations and variations, the
accumulation of variations from multiple
processes, to gauge tolerance. Tolerance should be
viewed in terms of what is required and not what
can be produced. Given enough time and money
almost anything can be produced.
Cosmetics
Cosmetic call outs can sky rocket the cost of metal
parts. Typically metal parts are categorized as
External (full view at all times in final product),
External/Internal - Both (partial view, or in full view
until fully assembled at customer sight), Internal (out
of view of customer), Structural or no cosmetic call
out required. Along with similar designations most
companies have developed their own inspection
criteria. Most are based on a viewing time and
distance with a maximum number of ‘flaws’ allowed
to be recognized within the allowable time at the
allowable distance. These specifications typically state
the criteria is primarily used to train inspection
personnel and can be used in determining accept or
reject decisions.
Cosmetics (cont.)
The shear nature of metal fabrication form the
handling of the raw materials to the equipment used
to the methods and processes used in fabrication are
all inherent with causing flaws or defects in material
surfaces. However fabricators and machine shops
have for years been producing products that meet
customers requirements. In some cases these ‘flaws’
are covered up by the finish of the part such as paint
or powder coating. But in some cases these ‘flaws’ are
accentuated by the finish of the part such as shiny
nickel or chem. film. Graining is required on many
higher cosmetic finish call outs. The graining process
does provide a more cosmetic finish but it does have
limitations. Graining or sanding is done early in the
process leaving many post processes that can and do
cause ‘flaws’. Also graining or sanding either
machined parts or sheet metal parts that have some
forming operations performed on the punch press can
not run through automatic sanding machines. Those
parts will either need special jigs made to carry the
parts through the sanding machine or be grained by
hand.
Cosmetics (cont.)
In addition the higher the
cosmetic call out the more
inspection time required
and the increase in scrap.
Most cosmetic
specifications differ only
slightly from one class to
another. There is very
little variation that can be
done in metal processes to
produce a part with two
flaws vs. four flaws. The
more stringent criteria
simply mean more
inspection and possibly
more fall out.
Cosmetic call outs are necessary to convey to the
manufacturers the desired results. It is however
cautioned that attention is paid to the actual use of the
part to determine if and when the extra money and effort
spent to achieve a higher cosmetic finish is necessary.
Closing
We hope you found this
presentation informative. The
intent was not to teach metal
design, simply to point out the
correlation between certain
design criteria and the
associated cost impact.
Thank you for your time!!!