Deep drawn stampings: design rules and failure modes

Deep drawn stampings are decided by two numbers, and both are calculated before anyone designs a tool. A 120 mm diameter cup drawn 60 mm deep in 1.2 mm CRCA starts as a 207.8 mm blank, which is a draw ratio of 1.73 and a single stroke on a 40 T press. Take the same cup to 90 mm deep and the blank becomes 240 mm, the ratio reaches 2.0, and the part needs two draws.

That is the fork in the road for every drawn part. One station is one tool, one press and one piece price. Two stations are two tools, an extra handling step and often an annealing decision, and the tooling difference is usually several times the piece price difference. A designer who calculates the ratio at the drawing stage chooses between those routes deliberately instead of discovering the choice during tryout.

The limits below are the ones we work to on 20–300 T mechanical presses, with the arithmetic shown so it can be checked. The failure modes that follow are the ones that account for most of the scrap we see on drawn parts, including the parts that arrive as a good drawing and a bad process.

What draw ratio decides whether deep drawn stampings need one stroke or two?

The first-draw ratio is blank diameter divided by cup diameter, and the practical limit is about 1.85 for CRCA in drawing quality. Above that limit the wall thins faster than the punch nose can carry the load, and the cup tears at the bottom radius.

The limit is a material property, not a shop preference. Austenitic stainless work hardens as it flows, so 304 sits lower at about 1.72. Annealed aluminium is softer but has less strain hardening reserve, so 5052 sits at about 1.65. Drawing-quality CRCA with a fine grain and a low carbon content reaches 1.85 to 1.9; commercial quality CRCA at the same thickness will fail closer to 1.7, which is why the grade callout on the drawing matters as much as the geometry.

The ratio converts to a reduction, which is how a tool room usually states it. A ratio of 1.85 is a 46% reduction in diameter, and 1.72 is 42%. Redraws are gentler because the material has already been worked: a second-draw ratio of 1.30–1.35 is normal, and a third draw is unusual on sheet below 3 mm.

Staging a cup that exceeds the first-draw limit

A 240 mm blank into a 120 mm cup is the worked case. The first draw cannot go straight to 120 mm, so the intermediate diameter is chosen to keep both stages inside their limits. At a second-draw ratio of 1.35, the intermediate is 162 mm, which makes the first stage 240 ÷ 162 = 1.48, comfortably inside 1.85, and the second stage 162 ÷ 120 = 1.35.

That staging matters for tooling cost. Two single-stage tools, two press setups and a transfer between them is the simple route. A compound or progressive tool that draws both stages in one stroke is faster but much larger, and it only pays above a volume where the cycle time saving exceeds the tool cost. We quote both and let the annual quantity decide.

Blank holder force is set from pressure over the area that is not yet drawn. On the 207.8 mm blank the sheet under the holder is the blank area minus the punch opening, or 33,914 − 11,310 = 22,604 mm². At 2.5 MPa that is 56.5 kN, which is 36% of the 158 kN draw force. Too little and the flange wrinkles; too much and the punch tears the bottom because the material cannot slide in. A nitrogen spring set is more repeatable than a rubber pad for exactly this reason: the force curve stays flat over the stroke instead of climbing.

Blank size and the tonnage calculation behind the press choice

Blank diameter for a cup with no flange is the square root of d² + 4dh, where d is the cup diameter and h is the cup height. For 120 mm and 60 mm the sum is 14,400 + 28,800 = 43,200 mm², and the root is 207.8 mm.

Trim allowance goes on top. A drawn cup rarely has a level top edge, so the blank is enlarged by 3–5 mm on diameter and the top is trimmed after forming. On the 207.8 mm blank that is a 212 mm blank, and the trim ring is scrap that has to be in the material calculation.

From the blank, three numbers follow:

• Blank mass. The blank area is 33,914 mm², which at 1.2 mm is 40,697 mm³, or 40.7 cm³ of steel at 7.85 g/cm³, so 320 g per piece before scrap.
• Blank layout. On a 1,250 mm coil with an 8 mm web, a 216 mm pitch gives five blanks across and a material utilisation of about 63%. A staggered layout buys a few points on a round blank and costs tool complexity.
• Draw force. Using the Siebel relationship, force is π × d × t × Rm × (blank ratio − 0.7). For 120 mm, 1.2 mm and 340 MPa that is 158 kN, or 16.2 tonne-force.

Draw force is not the press rating. The blank holder adds 20–30% on a part like this, so the working load is about 206 kN. Add a 30% margin for friction, material variation and tool wear, and the requirement is 27 tonne-force. The nearest press in the range is 40 T. A 20 T press would run the same job on paper and stall on the first coil with a harder temper.

Two side calculations are worth doing at the same time. Blanking the 207.8 mm circle in 1.2 mm CRCA at 240 MPa shear takes 188 kN, or 19 tonne-force, which already sits at the top of a 20 T press while the draw alone needs a 40 T. Piercing any holes in the same tool adds their own force, which is where the 250 T punching capacity on our larger presses becomes useful.

Draw and die limits by material

The table is the working set for a cup in the 100–150 mm diameter range. Values are for annealed sheet at the stated thickness; a harder temper or a thicker gauge moves the limit down, not up.

The five failure modes and the physical cause behind each

Most drawn-part scrap falls into five buckets. Each one has a cause that can be read from the part, which is what makes it fixable rather than a matter of opinion.

Tearing at the punch radius

The wall fractures where it passes over the punch nose, and the fracture is a dull shear band rather than a clean split. The cause is tensile stress exceeding the wall's remaining ductility: the ratio is too high, the punch radius is too small, the blank holder is too tight or the lubricant has broken down. Increasing punch radius is the cheapest fix and increasing the number of draws is the reliable one.

Wrinkling in the flange

The flange buckles because the circumferential compressive stress exceeds what the sheet can hold flat. Blank holder force too low, die radius too large or clearance too generous will each do it. A wrinkle that is ironed out in the die leaves a mark; a wrinkle that survives becomes a fold that cracks on the next draw.

Earing

The cup rim rises in waves because the sheet has planar anisotropy: yield strength and r-value vary with direction in the coil. Annealed CRCA typically ears 1–3% of cup height, and aluminium can ear more. Rotating the blank in the strip or trimming after the draw deals with it; changing the material is the expensive answer.

Galling and pickup

Metal transfers from the sheet to the die radius and then tears the surface it touches. Stainless is the usual victim because its passive oxide layer breaks down under pressure. The fix is a polished die radius, a lubricant with extreme-pressure additives, and a coating on the tool; running faster makes it worse.

Orange peel and stretcher strains

A coarse grain shows as a rough surface on the formed wall, and a yield-point elongation shows as Luders bands at low strain. Both are incoming material conditions, not tool conditions. They are why drawing-quality sheet is specified by grain size and why a change of coil supplier can change the surface of a part without any change to the tool.

What we run for drawn parts

Drawing runs on mechanical presses from 20 T to 300 T, with 250 T punching capacity for the blanking and piercing stations that share a tool with the draw. The tool room designs and builds the press tool, the blank holder and the checking fixture, and it maintains them for the life of the part, which is why a die that starts to wear is corrected on the machine that runs it rather than in a queue elsewhere.

A recent route for a drawn housing follows the standard sequence: blank on the press, draw in one station, trim the top edge, pierce the mounting holes, then deburr. Parts that need coating go through seven-tank pretreatment and powder coating on the same site, so the drawn surface is not handled between operations by a third party. First article inspection and PPAP documentation are available where the customer's quality system asks for them, and the general tolerance on formed features is ±0.5 mm unless the drawing calls something tighter.

Tooling is quoted separately from the piece price, and that is deliberate. A two-draw part carries two tools, and the buyer should see that number before committing to a volume that cannot amortise it. The press tonnage calculator will get you to the press class from the part geometry, and the stamping capability page sets out the rest of the route.

What to put on a deep drawing part drawing

1. Cup diameter, depth and corner radii, with the datum for depth taken from the inside face of the bottom, not the outside.
2. Material grade and temper, using the drawing-quality designation rather than "CRCA" alone, plus the thickness and its tolerance.
3. Draw direction or grain direction, if ear height or a visible feature makes it matter.
4. Wall thickness allowance, stated as a minimum, so the tool room knows how much thinning is acceptable at the die radius.
5. Trim allowance and the trimmed edge, including whether the top edge is a visible face after coating.
6. Hole positions relative to the drawn feature, with a positional tolerance and a note on whether they are pierced before or after the draw.
7. Surface requirement on the drawn wall, because a drawn surface shows handling marks and a cosmetic face needs a different lubricant and die finish.

A drawing with those seven items costs a few minutes to complete and removes most of the questions that otherwise arrive after the tool is cut. The drawn cups and housings guide covers the feature-level detail, and the deep drawing design rules covers the radius and relief decisions that sit around this calculation.

When deep drawing is the wrong route

Deep drawing is the right route when the part is a closed or semi-closed shell, the annual volume justifies a tool, and the wall has to be continuous. It is the wrong route in four common cases.

A part over about 400 mm in diameter, or deeper than about 250 mm in 2 mm steel, needs more tonnage than the 300 T top of our press range and a bed we do not have. A part that needs more than two draws in stainless usually needs interstage annealing, and that changes both the route and the lead time.

A part at low volume, under a few thousand pieces a year, rarely justifies the tool. Laser cutting and press-brake forming the same geometry in two or three pieces is often cheaper to first part and cheaper to change, even though the piece price is higher. The low-volume stamping guide sets out how to build a tool that survives that volume, and the press forming versus CNC bending decision covers the forming route that sits in front of it.

A part whose function is a flat panel with a stiffening rib is not a drawn part at all. It is a formed panel, and putting it on a draw tool adds cost without adding function.

If the part is a genuine shell, send the current revision with the material grade, the annual quantity and the surface requirement through the RFQ route, and the tool room will confirm the number of draws before the quotation is written. The rest of the drawn-part library sits under the stamping and press hub, including the catalogue of stamping defects that this article's failure section is built on.