Sheet Metal Design – What is a K-factor?

Introduction

One of the phenomena sheet metal fabricators must contend when bending parts is something called bending allowance. The reason for this is that when metal is bent, the material on the inside of the bend compresses, while the material on the outside stretches, and not by equal amounts (for reasons that get too technical even for this article). The result is that the workpiece actually “grows” in overall size if not compensated for. This compensation can be calculated using something called the K-factor, which considers variables such as the type of material, its thickness, the inside radius of the bend, and how it is bent.

What does this mean to the part designer? Even if your part is designed as a sheet metal part in a CAD Solids Modeler, when flattened, the flat development may or may not be correct, depending on the above-noted variables. It is for this reason that reputable metal fabricators may revise the model, and add their particular press brake bending parameters to create an updated flat development that will yield the part you require, and within your required tolerances.

Knowing your fabricator’s process and press brake tooling available (notably the radius of the male break dies), goes a long way to save time and potential surprises. The purpose of this article is to demonstrate to engineers and designers the technical aspects of how we (and you!) can determine the K-factor in sheet metal design.

Problem Statement

When files are provided by the customer, the 3D model has no bending parameters specified if it’s a STEP, IGES, or Parasolid file, and bending parameters are set to a default value in SolidWorks. When the flat pattern is developed for the part to be cut, it will often have incorrect dimensions to yield the customer’s desired bent part. In order to overcome this problem, your sheet metal fabricator should calculate the K-factor and revise the part’s flat development to yield your desired part within your specified tolerances.

Why is K-factor important in sheet metal manufacturing?

The K-factor in sheet metal design is important since it is used to correctly calculate flat patterns. This is because it is directly related to how much material is stretched during bending. K-factor is the ratio of the neutral axis to the material thickness. K-factor plays a key role in understanding the limits a material can handle during sheet metal bending.

General equation for K-factor:

BA= Bend Allowance

μ= Material Thickness

ρ = Inside Radius

β = Bend Angle (in degrees)

Calculating K-factor

1. Measurements taken from a bracket we manufacture:

β = 90°
ρ = 0.142 in (see Fig. 1)
μ = 0.135 in (Hot Rolled Steel)

FL1 = 1.378 in (see Fig. 2)
FL2 = 1.462 in (see Fig. 3)
Initial length = 2.583 in (see Fig. 5)

FIG. 1
Fig. 2
FIG. 3

2. Now that you have your measurements, we’ll determine the BA. To do this, first determine to bend outside set back (OSSB)

OSSB=Tan (β/2)(ρ+μ) Tan (90/2)(0.142+0.135)
OSSB = .277 in
FIG. 4
FIG. 5

Then determine the bend deduction (BD is not part of the formula but can be used instead of the K factor if desired).

BD = FL1 + FL2 – Initial length

3. Calculate bend allowance using the following equation

BA = 2*OSSB
= 2* 0.277
= 0.297 in

4. Plug the Bend allowance (BA), the Bend Angle (β), Inside Radius (ρ), and Material Thickness (μ) into the below equation to determine the K-factor (K).

Conclusion

A practical method to calculate the K-factor

1. PREPARE SAMPLES

- Begin by preparing 5 sample blanks which are of equal and known sizes .
- Record material type and thickness in test report
- The blanks should be at least a foot long to ensure an even bend, and a few inches deep to make sure you can sit them against the back stops.
- Measure Initial length of metal blank

2. BEND TESTING

- Set up the press brake with the desired tooling you’ll be using to fabricate this metal thickness. Make sure to use the same die and punch for all samples. If different punch or die is used it needs to be mentioned in the test report.
- Place a 90° bend in the center of the piece.

3. MEASURE SAMPLES

- Measure the flange length and inside radius of each piece, record length A,B and radius R as shown in the Fig. 6.
- The test report should have material type, material thickness, initial blank length, inside radius, flange length A and B at this step.

4. CALCULATION

- Calculate the K-factor by following the procedure mentioned earlier with the measurements obtained.
- This K-factor value is to be used in the trail-and-error approach in the following steps.

5. MODELLING

- Use the flange lengths measured to create a model on SolidWorks as shown in Fig. 7 and set the K-factor value obtained from the calculation (Step 4) in the SolidWorks model.

6. VERIFY

- Finally, develop a flat pattern from the model, and adjust the K-factor in SolidWorks until the flat pattern dimensions are equal to the measured initial length of the metal blank. The right K-factor of the metal that is being tested is when the overall flat pattern dimensions are equal to the measured initial length of the metal blank.

FIG. 6
FIG. 7

TriparTech: Design for Manufacturability, Part 2

Part II: Feature Design

As a metal fabricator, we see designs which are complex, but when analyzed, have few inherent features that are difficult to realize. The result is what all OEMs want; a design which meets their requirements for the lowest possible part cost, with consistent results from the fabricator. All too often, OEMs have not considered Design for Manufacturability (DFM), (or to the degree they should), only to see quotes that are far higher than they anticipated, or worse, no quotes due to inherent impossibilities.

Another reason for lack of DFM could be due to the Designer’s perception of how the part will be manufactured. It could be that since initial volumes may be on the lower end, the designer is thinking of the part being made by flexible manufacturing processes, such as CNC laser, punching and bending, designing the part as such. Exploiting the capabilities of these incredible machines is often a great starting point; to look at the capabilities please download our CNC Punch/Laser Design Guide.
However, as volumes increase, hard tooling may offer more economical solutions. If the Designer did not consider how the same part might be hard tooled, (made in one or more dies), it may prevent the part from being hard tooled, even as higher volumes might dictate, or not without design changes.

Whether the part will be made by flexible manufacturing processes such as CNC Laser, punch and bending, or hard tooled in progressive dies, the design principles remain the same. Based on our experience as both a metal stamper & fabricator, the following are many examples of do’s & don’ts to achieve DFM:

1. DON’T place holes/slots too close to one another. Minimum edge to edge distance between hole/slots is recommended to avoid metal distortion, deformation and fracturing. In the case of die stamping, if two adjacent holes/cut-outs are too close to one another, there will be insufficient strength in the bridge between the two for the tool steel to withstand the punching forces. There are ways around this, such as punching one hole in one station, then advancing the material to another station where the second is punched (with the holes still ending up adjacent to one another). Since the two holes within the die are now separated, there is sufficient tool steel around each hole. However, this is also achieved at a cost, since the die is now longer, and possibly a new station has been added that might otherwise not have been required if the separation between holes or features was greater.
As a rule of thumb, and as shown in figure 1, try to keep the distance between holes (the distance from closest edge to closest adjacent edge) at least 2 times the material thickness, and preferably 3 times.

Figure 1: Minimum distances between holes or cut-outs.

2. DON’T place holes/slots too close to the bend edge. For example, whether a short upward bend needs to be next to a hole or cut-out, keeping a minimum distance between them will solve what could otherwise lead to distortion, deformation, fracturing and other problems. For example, with CNC punching, if an upward bend is too close to a punched hole, the upper die head in the CNC punch press could interfere with the bend, necessitating an extra operation at added cost.

As a rule of thumb, keep a minimum distance between the bend and the closest edge of the hole/slots 2 times material thickness plus the bend radius (dimension “S” below).

Figure 2: Minimum distance between holes and bends.

3.  DON’T have bends too close to the edge of the material. Say for example, a .09” high bend is desired near the edge of a piece that is made from .06” thick sheet. As shown in figure 3, there is much more material being supported in the V-die on one side than the other.

Figure 3: Imbalanced bending due to short leg.

This leads to unbalanced frictional forces, which often lead to either an incomplete bend, or a bow in the material. If a smaller V-die is used, so the same amount of die material is in contact with the sheet on both sides of the bend, the forces required to achieve the bend will rise, may still not prevent bowing, and may leave die marks on the outside of the bend due to the higher forces.

As a rule of thumb, and as shown in figure 4, try to have the shortest wall or leg in any bend at least equal to 3 times the material thickness plus the bend radius.

Figure 4: Minimum wall/leg height.

4. DON’T specify a tighter than necessary bending radius. As mentioned in DFM I, Tolerance Tolerant Designs, radii should be specified to the inside of bends or forms, as the outside is not as controllable, and is also affected by the material thickness tolerance.  In addition, inside bend radii should ideally be equal to material thickness as shown in figure 4; less, in some cases will lead to various problems, including cracking on the outside of the bend and necking. Keeping the bend radius constant throughout the design can also increase the chances of allowing using same tool to be used through the bending process, potentially reducing set-ups, operations, and cost.

5. DO choose the minimum hole diameter that reduces punch loading and excessive burr. Keep in mind that small size punches are more prone to failure. Therefore the minimum hole diameter should never be less than the material thickness, and sometimes 2 times the material thickness for harder materials, as shown in figure 5. If for some reason the hole diameter must be less than the material thickness, it may be laser cut, but the required tolerance may not be achievable. For example, in the case of holes requiring a small PEM insert to be pressed in, the required hole tolerance is often +.003/-.000; something that may be not be achievable by laser cutting.

Figure 5: Minimum hole diameter.

6. Bend relief must be provided at the end of bent edges that meet, in order to  avoid “overhangs” and tearing at bends. Overhangs become more prominent for thicker parts with smaller bend radii, and may even be as large as one half of the material thickness. Bends made too close to an edge may also cause tearing. As a rule of thumb, bend relief must be at least equal to the material thickness in width “W”, and be longer “L” than the bend radius, as shown in figure 6.

Figure 6: Bend relief before and after bending.

Conclusion

Remember that features and feature complexity correlate directly to part cost. Always try to simplify (or eliminate!) as many features as possible. If in doubt, ask your fabricator.

There are a great many ways in which to manufacture a part. Besides telling your fabricator the lot quantities you would like quoted, also try to give them your EAUs. They know their equipment, so they should be in a position to solve your problem for the lowest possible cost given the lot quantities and EAUs.

As noted in DFM I, if you are unsure, share your assembly with your fabricator. One who works in your interest, and understands and applies the techniques of DFM, may have cost-saving solutions for you.

For more information please contact TriparTech@TriparInc.com.

TriparTech: Design for Manufacturability, Part 1

To download the PDF of our newest TriparTech: Part I, Tolerance Tolerant Designs, please click here.

Part I: Tolerance Tolerant Designs

As a metal fabricator, we see designs and drawings from a huge range of OEMs. Some of these are well thought out with sensible tolerances, and follow sound practices of Design for Manufacturability (DFM). Others have arbitrary or ill-though out tolerances, or strictly use default tolerances, all of which adds complexity to the manufacturing process, resulting in higher parts prices than would otherwise be necessary.

Perhaps some Designers feel that precision = quality. This is a falsehood, and nothing could be further from the truth. Quality is in fact a part that consistently meets specifications, whose tolerances are neither precise (tight) nor loose, but functionally appropriate for the assembly in question. Generally, the wider the tolerances that can be applied, with tighter tolerances applied only if/where required, will yield a quality part that meets both the drawing specifications and application, and for the lowest possible cost! This is the first step toward DFM.

Based on our experience as both a metal stamper & fabricator, the following are many examples of do’s & don’ts:

1. DON’T arbitrarily apply the default tolerance table that is present in most drawing templates! For example, if it is as shown in Figure 1a below, and most features of your part do not require such tight tolerancing, change the table as shown in Figure 1b!

Figure 1a. Original Table

Figure 1b. Modified Table

Conversely, there may be instances when you must tighten up the default tolerance for very stringent applications. If that is required, then so be it, but remember that this often drives up cost. You do not have to worry if your drawings do not all contain the same default tolerance table. It is up to the manufacturer to read and respect these and all requirements noted.

2. DON’T forget about default angular tolerance in the same table. These often state  ANGLES ± 1/2⁰ (or ± 30’). This translates to only 0.009” over a 1”! If your part only needs ± 1⁰ or ±2⁰, change it!

3. DON’T rely solely on the default tolerance table! Besides specifying the tolerance based on the number of decimal places, the same table almost always states UNLESS OTHERWISE SPECIFIED. Even if you have modified your default tolerance table (as suggested in points 1 & 2 above), there may be features that can afford greater tolerances (that may otherwise be cost-drivers). If so, override (..OTHERWISE SPECIFY…) the default tolerance by adding the more relaxed tolerance right after the dimension. Figure 2a below shows a dimension of 2.875, which in the case of the associated default tolerance table, would carry a tolerance of ± .005”. If in fact this is not only tighter than necessary, but say that it can also never be below 2.875, override the default tolerance by adding only what is required; e.g. the same 2.875 dimension, but with a wider +.03/-.00 tolerance, if that is what the part and eventually assembly require.

Figure 2a. Dimension riding on default tolerances.

Figure 2b: Dimension with tolerance that overrides the default tolerances.

The same principle applies if there is a dimension that requires a tighter tolerance than what the default tolerance table permits; override it as required!

4.  DON’T dimension to theoretical points. For example, 4.21. Instead, try to dimension to physical features that are easily measured on the part.

Figure 3a.

Figure 3b.

5. DON’T dimension to features that are not in line with one another unless necessary. For example, Figure 4a below shows the relative position of two knockout holes to one another. Being offset in both directions can make it difficult on the factory floor for the fabricator to check this. Considering that the relative position of two adjacent knockouts is rarely critical, an simpler dimensioning scheme is shown in Figure 4b below, where the position of both holes is independent and referenced from edge that are adjacent to both.

Figure 4a: Relative dimensioning

Figure 4b: Independent dimensioning

6. DON’T specify near perfection on flatness, as nothing is ever perfectly flat. Instead, try to bias your flatness tolerance to allow a maximum curvature in one direction, so that the part will flatten upon assembly, or even become a feature! For example, the driver box covers shown below are intentionally curved so that once the tab at one end is placed into a receiving slot in the box, the cover will “unroll”, or flatten itself until the free end is snapped and held by a retaining spring.

Figure 5: Curved cover flattening upon installation

This ensures that the cover makes intimate contact with the top edges of the box. Installed the opposite way would leave a bowed cover and a gap in the middle. With a smart design, this however is impossible as the tab at the end is off-center, forcing it to be oriented prior to installation, with the curvature in the intended direction!

7. DO be aware that every bend adds complexity, and a dimension & tolerance that is dependent on the precision of two or more bends, becomes increasingly difficult to achieve. Figure 6a below shows a somewhat tall yoke (U-shaped) bracket with an inside dimension and tolerance of 5” ± .06”, (which as dimensioned, applies over the entire height of the part). The ± .06 tolerance may seem generous, but over a 10” height, if the bottom is at the lower limit of this (4.94”), and the top end at the upper limit (5.06”), that results in an angular difference per side of only 0.3⁰!

Instead, think about the application. Often the upper, or “free” ends of the yoke is intended to secure something that fits or is secured within it, at which point the arms should appear to be nearly parallel.

Figure 6a: Arbitrary dimension & tolerance applied over full height of yoke

Figure 6b: Tight tolerance applied to bend area, with generous tolerance to arms

A way to achieve this at potentially lower cost is shown in Figure 6b, which specifies that the 5” ± .06” dimension only applies where the radius at the closed end finishes, but that the free end may be more generous at 5” ± 0.25”. Sure, the arms may appear dreadfully non-parallel upon receipt from the fabricator, but have a better chance of being within a far more cost-effective tolerance, yet when assembled with whatever fits within the free ends, will end up being parallel! Or, if you want the part that fit within the arms to always have light to moderate pressure, bias the tolerance, while still keeping it generous, e.g. 4.98” +0.00/-.25”.

Now imagine a similar yoke, but one which has two more bends as shown in Figure 7a. Here, the upper or “free” end dimension of the yoke is determined by four bends. Achieving a tight tolerance in this case is even more difficult to achieve, and even more costly if an arbitrary tolerance is given without thought to the manufacturing difficulties involved. Apply the same strategy as explained above to keep costs down without any compromise to your overall assembly!

Figure 7a: Tight dimension & tolerance applied only to the free end opening

Figure 7b: Where possible, tighter tolerance applied to bend areas, with no tolerance to the free end opening

8. DO remember that all sheet materials have a thickness tolerance, which are also different amongst materials. For example, cold-rolled steel (CRS) and galvanized steel may be offered in the same gauges, but they each come with different tolerances. Similarly, some materials are not bought in gauges, but in nominal thicknesses (e.g. aluminum and stainless steel). See table below. Make sure that your design, drawing, and tolerances can cope with these material tolerance variations!

Gauge  HR Steel HR Tol  CR Steel CR Tol Galv Steel Galv Tol Stainless Steel SS Tol Aluminum Alum.Tol
3 0.2391 +/-.009 0.2391 0.25 0.2294 +/-0.011
4 0.2242 +/-.009 0.2242 0.2344 0.2043 +/-0.011
5 0.2092 +/-.009 0.2092 0.2187 0.1819 +/-.009
6 0.1943 +/-.009 0.1943 0.2031 0.162 +/-.009
7 0.1793 +/-.008 0.1793 +/-.008 0.1875 +/-.007 0.1443 +/-.007
8 0.1644 +/-.008 0.1644 +/-.008 0.165 +/-.007 0.1285 +/-.007
9 0.1495 +/-.008 0.1495 +/-.008 0.1532 +/-.009 0.1562 +/-.007 0.1144 +/-.006
10 0.1345 +/-.008 0.1345 +/-.006 0.1382 +/-.009 0.1406 +/-.006 0.1019 +/-.006
11 0.1196 +/-.008 0.1196 +/-.006 0.1233 +/-.009 0.125 +/-.005 0.0907 +/-.0045
12 0.1046 +/-.008 0.1046 +/-.006 0.1084 +/-.009 0.1094 +/-.005 0.0808 +/-.0045
13 0.0897 +/-.007 0.0897 +/-.005 0.0934 +/-.008 0.0937 +/-.004 0.072 +/-.004
14 0.0747 +/-.007 0.0747 +/-.005 0.0785 +/-.008 0.0781 +/-.004 0.0641 +/-.004
15 0.0673 +/-.006 0.0673 +/-.005 0.071 +/-.006 0.0703 +/-.004 0.0571 +/-.0035
16 0.0598 +/-.006 0.0598 +/-.005 0.0635 +/-.006 0.0625 +/-.003 0.0508 +/-.0035
17 0.0538 +/-.006 0.0538 +/-.004 0.0575 +/-.005 0.0562 +/-.003 0.0453 +/-.0035
18 0.0478 +/-.005 0.0478 +/-.004 0.0516 +/-.005 0.05 +/-.003 0.0403 +/-.003
19 0.0418 +/-.004 0.0418 +/-.004 0.0456 +/-.005 0.0437 +/-.003 0.0359 +/-.003
20 0.0359 +/-.003 0.0359 +/-.003 0.0396 +/-.004 0.0375 +/-.002 0.032 +/-.0025
21 0.0329 +/-.003 0.0329 +/-.003 0.0366 +/-.004 0.0344 +/-.002 0.0285 +/-.0025
22 0.0299 +/-.003 0.0299 +/-.003 0.0336 +/-.004 0.0312 +/-.002 0.0253 +/-.002
23 0.0269 +/-.003 0.0269 +/-.003 0.0306 +/-.004 0.0281 +/-.002 0.0226 +/-.002
24 0.0239 +/-.003 0.0239 +/-.003 0.0276 +/-.004 0.025 +/-.0015 0.0201 +/-.002
25 0.0209 +/-.003 0.0209 +/-.003 0.0247 +/-.004 0.0219 +/-.0015 0.0179 +/-.002
26 0.0179 +/-.002 0.0179 +/-.002 0.0217 +/-.003 0.0187 +/-.0015 0.0159 +/- .0015
27 0.0164 +/-.002 0.0164 +/-.002 0.0202 +/-.003 0.0172 +/-.0015 0.0142 +/- .0015
28 0.0149 +/-.002 0.0149 +/-.002 0.0187 +/-.003 0.0156 +/-.0015 0.0126 +/- .0015
29 0.0135 +/-.002 0.0135 0.0172 +/-.003 0.0141 0.0113 +/- .0015
30 0.012 +/-.002 0.012 0.0157 +/-.003 0.0125 0.01 +/- .0015
31 0.0105 0.0105 0.0142 0.0109 0.0089 +/- .0015
32 0.0097 0.0097 0.0134 0.0102 0.008 +/- .0015
33 0.009 0.009 0.0094 0.0071 +/- .0015
34 0.0082 0.0082 0.0086 0.0063 +/- .0015
35 0.0075 0.0075 0.0078 0.0056 +/- .0015
36 0.0067 0.0067 0.007

9. DO remember that when parts are bent or formed, they are usually “wrapped” around a male die. As a result, dimensions should be to the inside of such radii or forms, as the outside is not as controllable, and also affected by the material thickness tolerance or variations.

10. DO try to give as much latitude on bending radii as possible, as this will increase the chances that your fabricator can find a suitable bending die within his arsenal of press break tooling. If not, you, the OEM, are going to pay for that new bending die; either up front, or it will be buried in the fabricator’s quote.

For example, if you are designing with 16 GA CRS (0.06”), and have called for an inside radius of 0.12 (smartly adhering to the rule of thumb that inside radii should never be less than 1.5 times material thickness, or preferably 2 times the material thickness), but you can live with an inside radii up to 0.18”, specify the radii as 0.18/0.12”. This increases the chances that you fabricator will have existing dies within the range. And don’t worry if your flat development was designed for a 0.12” radius. If you fabricator wishes to use a 0.18” radius, it is up to them to modify the flat development to yield the bent part. After all, what you are purchasing is generally the bent or formed part, which is what your supplier must respect.

11. DO remember that if a metal stamping or fabricated metal part is what you have designed, that by the very nature of the process, there will be slightly sharp edges and small burrs. Specifying PART SHALL BE FREE OF BURRS, or worse, DEBURRS AND BREAK ALL SHARP EDGES, will always drive up cost! Small burrs are a nature of the process, thus fabricators will often state on their quote PART SUPPLIED IN ITS AS STAMPED CONDITION. If this is an issue, it is up to the OEM to discuss this further with the incumbent supplier.

If this is absolutely required, there are ways it might be achievable, but at increasing cost. Small parts that are also not subject to permanently flex upon light loads may be able to be tumbled or vibratory finished. This may soften the outer edges of the part, but depending on the deburring process and media used, it may not deburr within tight corners or small holes & cut-outs. Larger and more fragile parts may need to be run through a timesaver (part passed through a sandwich of two wide flat abrasive belts), or hand manipulated to deburr edges against an abrasive belt or wheel. However, all of these are extra steps, adds cost, and may also affect or change the surface finish in unpredictable and often non-repeatable ways.

The best solution to this is to work with a reputable fabricator who will monitor all tools for wear, thus keeping burrs to a minimum.

Conclusion

Remember that relying on a drawing’s default tolerance table may save you design time, but if it results in an overtoleranced (or ill-toleranced) part that may not work within your assembly, the initial savings in reduced design time will often be wiped out on recurring part costs, for which there may be many thousand/hundreds of thousands produced over many years!

Think about how you parts will ultimately be used, dimensioning and tolerancing appropriately, remembering that large tolerances do not equate to low quality. In fact, a well dimensioned and toleranced part equates to quality in that it will yield the part you need for the application; no more and no less, while having the greatest potential to save part cost.

You, the OEM knows how each part is used in your assembly, thus you are best placed to give time and consideration to tolerancing. If you are unsure, share your assembly with your fabricator. One who works in your interest, and understands and applies the techniques of DFM, may have cost-saving solutions for you.

Watch for Part II – Feature Design in an upcoming issue of TriparTech.

For more information please contact TriparTech@TriparInc.com.

TriparTech: Drawing & Deep Drawing

Drawing & Deep Drawing

Drawing is a sheet metal forming process used to create three dimensional forms from a single blank with no overlaps, seams, or other means of the part retaining its formed shape.

A sheet metal blank is radially “drawn” into a forming die or over a rigid post, by a mechanical or hydraulic press into a seamless can, or other shape, e.g. sinks, gas tanks, housings for engine oil filters, and pots and pans.

Either a pre-cut round blank is placed in the draw die, or coil is fed through a compound draw die, and the required round blanked   at the very instant before drawing begins. The blank diameter is pre-determined by calculation and /or experimentation. The blank’s flange region, the outer area of the blank (exclusive of the draw opening) experiences a radial drawing stress and a tangential compressive stress due to the material retention properties.

Imagine the part being drawn as the hub of a bicycle wheel and the spokes representing the forces being applied to the flange as the drawing takes place, as shown in the image below. Unrestrained, these compressive stresses would result in what is known as “flange wrinkles”. These can be prevented by using a blank holder, the function of which is to control material flow as the part is drawn.

Please watch the video below to know more about Draw and Deep Draw.

Please click here to watch more Tripar’s videos on our YouTube channel.

Other operations such as punching and flange trimming can sometimes be combined with the drawing process.

Deep Drawing Process

Where the height of the part approaches or exceeds its diameter or minimum part width, the process is known as deep drawing. This is achieved by redrawing the part through a series of dies or “redraw” operations, whereby material is taken from the top, and reformed and slightly stretched to provide the additional depth required (shown in 0:17 -0:37 in Draw and Re Draw video above).

The photos show the re-draws required to make an aluminum shell 6” dia. x 11” high from an 18-1/8” diameter blank.

Deep Draw metal stamping Materials

Many different metals can be deep drawn. Cold rolled steel, stainless steel, copper, brass, aluminum, and others are possible using the deep drawn stamping process.

The four principle classes of available low-carbon sheet/strip steel are Commercial Steel (CS), Draw Steel (DS), Deep Draw Steel, (DDS), and Extra Deep Draw Steel (EDDS) also referred to as IF or Interstitial Free steel, each of which has increased “draw-ability”, but also at increasing cost.

The following principle factors affect the selection of grade and quality of low-carbon steel sheets and strip for deep drawing.

  1. Severity of draw as determined by the amount of reduction.
  2. Thickness of the material.
  3. Shape of the part (round, rectangular, or conical)
  4. Flange requirements
  5. Ironing requirements
  6. Desired finish
  7. Grain size
  8. Press speed
  9. Availability of material
  10. Cost

Deep Drawing Presses

A variety of deep draw presses, each of which have different capabilities, are used to produce deep drawn metal stampings.

Either mechanical or hydraulic, the press requires the tonnage or force required to draw the part. Ram speed is another determinant for deciding which tonnage press is most suitable, which must not exceed the draw speed of the material. The press also needs to be equipped with a die cushion which is usually located below the press bed, the purpose of which is to provide pressure on the blank holder in order to control material flow over the die radius; too little pressure can result in wrinkles, while too much pressure can restrict material flow to the point where cracking or tearing occurs.

Deep Drawing Station Types

The deep draw stamping process consists of many smaller individual processes. These can include the following:

  • Blanking: Blanking is the process of cutting the initial sheet or coil stock into round or shaped flats required for deep drawing.
  • Drawing: Drawing is the process of forming the metal with a punch and die, and is the heart of the deep drawing process. Drawing is often accomplished with a progressively smaller series of dies that reduce the shape and increase depth of the part.
  • Blanking and Drawing: Combines the blanking and drawing operations in a compound die.
  • Piercing: Piercing is the process of punching holes in the metal stock that are required for the finished part.
  • Trimming: In the Trimming process, excess metal that is necessary to draw the part is cut away from the finished part.

When quantities warrant, deep drawn parts are made in a progressive die where the part is carried on a steel web as shown in the photo.

As the material progresses through the die and forming process, the part may receive additional operations such as:

  • Beading: Material is displaced to create a larger, or smaller diameter ring of material beyond the original body diameter of a part, often used to create O-ring seats.
  • Bottom Piercing: A round or shaped portion of metal is cut from the part.
  • Bulging: A portion of the part’s diameter is forced to protrude from the surrounding geometry.
  • Coining: Material is displaced to form specific shapes in the part.
  • Curling: Metal is rolled under a curling die to create a rolled edge.
  • Extruding: After a pilot hole is pierced, a larger diameter punch is pushed through, causing the metal to expand and grow in length.
  • Ironing: A process to reduce the wall thickness of parts.
  • Necking: A portion of the part is reduced in diameter to less than the major diameter.
  • Notching: A notch (round, square, or shaped) is cut into the open end of the part.
  • Rib Forming: Involves creating an inward or outward protruding rib.
  • Side Piercing: Holes are pierced in the side wall of the drawn part.
  • Stamping / Marking: Typically used to put identification or markings on a part.
  • Threading: Using a wheel and arbor, threads are formed into a part.
  • Trimming: Excess metal that was necessary to draw the part is cut away from the finished part.

Comparison of Drawing & Deep Drawing to Metal Spinning:

Advantages:

  1. Surface finish: As opposed to metal spinning, which often leaves a poor surface finish containing what is known as “spin marks”, the draw and deep drawing process usually leaves a much finer and consistent finish.
  2. Precision: Drawn and deep drawn parts typically have less dimensional variation and much tighter part tolerances.
  3. Shape: Spinning is limited to round shapes, whereas a deep drawn part can be square, rectangular, or a mixture of profiles (e.g. gas tanks), subject of course to the stress & strain limits of the material being used and the desired shape.
  4. Part cost: Due to the much faster production rates over metal spinning, a drawn part will almost always cost less.

Disadvantages:

  1. Tooling Cost: Draw dies, depending on their complexity, can become quite costly, the justification of which is based on projected volumes, as well as if/what other alternatives there may be.

Conclusion

Working with a reputable and experienced metal stamper having drawing and deep drawing experience and existing tooling, is your best chance to capitalize on using this process. Remember, the more flexibility you have with your design, the greater the likelihood of reducing the number of redraws required, as well as capitalizing on that manufacturers existing tooling, potentially with minimal tooling modification.

For more information please contact TriparTech@TriparInc.com.

TriparTech: Progressive Dies & Progressive Die Stamping

Overview

Progressive die stamping is a sheet metal forming process widely used to produce parts for a variety of industries. Progressive dies contain individual work stations, each of which performs one or more different operations on the part, such as piercing, blanking, coining bending, forming, and even drawing. The precision components within the progressive die are mounted within what is known as a die set (a heavy steel upper and lower plate with precision guide pins to align the two plates), which is placed into a reciprocating stamping press. As the press moves up, the upper die half moves with it, allowing the material to feed or advance with each stroke. When the press moves down, the die closes and performs the stamping operation, simultaneously at all work stations.

A feeder or feeding system typically pushes a strip of metal (usually from a coil) through all of the stations of a progressive stamping die at a specific distance or “pitch”, which is a constant distance between each station within the die. As the strip is pushed through the die, each station performs a specific operation. As the strip progresses, an increasing number of features become inherent within the part. The final station is a cutoff operation, which separates the finished part from the strip or carrying web. With each stroke of the press, a completed part is removed from the die. The carrying web, along with metal that is punched away in previous operations, becomes scrap metal. Both are either knocked through or cut away from the die, and then ejected from the die set.

Since additional work is progressively done in each “station” of the die, it is important that the strip be advanced very precisely so that it aligns within a few thousandths of an inch as it moves from station to station. Tapered or conical “pilots” enter previously pierced holes in the strip to ensure this alignment, since the feeding mechanism alone cannot usually provide the necessary precision in feed length.

The high precision die components (die blocks, punches, cams, etc.) are usually made of heat-treated tool steel to withstand the high shock loads, to retain a sharp cutting edge, and to resist the associated abrasive forces.

Financial Considerations

Progressive dies costs are determined by part’s complexity, the number of features, and the complexity of each feature. Minimizing and simplifying all of these aspects within the part, will keep tooling, or die costs to a minimum. Features that are small, narrow, or close together can be come problematic because there may not be sufficient clearance, requiring additional die stations, all of which drives progressive die costs.

Progressive die costs range from under $10,000, to upwards of hundreds of thousands of dollars, and are most dependent on part size and complexity. Justification for a progressive die is almost always dictated by part quantity. Given sufficient volume, progressive die stamping may be justified as the process leads to the lowest part cost, largely due to high production rates, thus relatively low labour cost per part, and often no secondary operations.

Alternatives

Alternatives to progressive die stamping include;

  • CNC Punch, laser, and other metal fabrication techniques: These require little or no tooling, thus are ideal for lower part volumes. However, because of increased material and part manipulation, operations, and labour, part cost will invariably be higher.
  • Partial Progressive: This is where some of the part features are produced in a progressive die, but the most
    complex features, or those which have multiple variants, are produced either in a secondary (and lower
    cost) die, or finished or customized using CNC metal fabrication techniques.

Progressive die stamping is explained in the following Tripar video:

Please click here to watch more Tripar’s videos on our YouTube channel.

Conclusions

In conclusion, unless part quantities are exceptionally high (where a progressive die is likely the best solution), or exceptionally low (where a non-tooled solution may be warranted), a cost/benefit analysis must be performed to assess the short to long term costs at different volumes using each process. Working with a reputable metal stamper/fabricator that offers multiple processes & solutions will help determine the optimal solution for you.

For more information please contact TriparTech@triparInc.com.