H & S Manufacturing Co.

H&S Manufacturing Co. contract manufacturing Expertise $ Cost Drivers $ Innovation Experience Correlations between DESIGN & COST in precision metal

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 PRINTS NOTES SPECFICATIONS 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.) 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. Tolerance Summary(cont.) 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!!!

H & S Manufacturing Co.