What this page settles. 1) Which tool carries the size of a blanked outline and which one carries the size of a pierced hole. 2) Why the same clearance figure is added in one case and subtracted in the other, and what a wrong reading costs. 3) Why burr direction follows punch travel rather than the name of the operation. 4) How to split a single tolerance band between an outside edge, a hole and the part that mates with it.
Two cutting edges meet the same sheet during one press stroke. One of them runs around the outside of a bracket, and the other punches a hole inside it. Both cuts shear metal, both throw off scrap, and a quotation usually lists them under one heading. Trouble begins when a drawing treats them as one family of tolerances, because the two cuts do not hold size in the same way.
Blanking and piercing are separated by what leaves the press as the product:
1) Blanking keeps the piece that comes out. The cut defines the outer contour, and the strip left behind becomes the skeleton that goes for recycling.
2) Piercing keeps the piece that stays. The strip continues down the line as the part, and the material pushed through the die is the slug.
3) Both cuts produce a slug. Ownership is the difference, not mechanics: one slug is the part, and the other is waste.
Ownership reaches further than most designers expect. A pierced hole is measured as an internal feature, so a pin gauge, a plug gauge or a CMM probe reaches it from either face. A blanked outline is measured as the boundary of the part, and the operator sees it as the line where the strip separates. Same stroke, two inspection habits, two sets of instruments, and two different arguments when a lot comes back rejected.
Once the part leaves the die, the difference keeps showing up. Hole diameter, hole position and flatness sit on a first article report as separate line items, while a blanked outer edge is usually checked as a general size rather than as a located feature. Reading those two lines as interchangeable is where suppliers and buyers begin to disagree about who owns a dimension.
Blanking carries a cost that piercing does not. Every blank consumes the strip around it, so the skeleton between parts is bought and scrapped, while a hole pattern adds almost nothing to material cost. A quotation that moves when holes are added is rarely moving because of the holes.
Size is created by whichever cutting edge stays with the dimension. In piercing, the punch passes through the sheet and the hole takes the punch diameter, so the die opening has to be larger than the punch by the full clearance. In blanking, the part falls through the die opening, so the die opening decides the outside size and the punch has to be smaller. Two operations, one rule, and the rule runs in opposite directions.
| 01Piercing: the punch carries the size. A 6.00 mm hole needs a 6.00 mm punch, and the die opening is built larger by the total clearance. The hole is a copy of the punch, made once per stroke, for the life of the tool. | 02Blanking: the die opening carries the size. A 60.00 mm outline needs a 60.00 mm die opening, and the punch is cut smaller by the full clearance. The part is a copy of the die opening, which makes the female side the expensive one to change. |
| 03Wear pushes the two dimensions apart. The punch loses material and the pierced hole drifts smaller. The die opening wears open and the blanked outline drifts larger. Both effects grow with stroke count, and neither one reverses on its own. | 04Replacement cost is not symmetrical. A worn punch is a ground or replaced insert. A worn die opening is a welded, re-cut or replaced block, and that work reaches into the die structure instead of sitting on top of it. |
That asymmetry suggests a placement rule for anyone writing the drawing. Put the tight band on the dimension that matters for function, and expect the loose band to be consumed by tool wear rather than by the first part off the press. A first article sitting in the middle of a hole tolerance will drift toward the low limit as the punch wears, and one sitting in the middle of an outline tolerance will drift toward the high limit as the die opening wears.
Designers who have been through a few tool life cycles write one-sided tolerances for exactly this reason. A pierced hole behaves better as 6.00 mm plus 0.05 mm than as 6.00 mm plus or minus 0.05 mm, because the direction of travel is known in advance. The same logic applies to a blanked outline, where the useful band sits below nominal.
Clearance is the gap between the punch edge and the die edge, and it is normally written as a percentage of material thickness per side rather than in millimetres. The percentage carries the intent, and the thickness turns it into a number the tool room can grind to. A 1.0 mm sheet at 6 percent per side gives 0.06 mm at each cutting edge, which is a normal working figure on mild steel and roughly a tenth of the sheet thickness itself.
Published recommendations move with the grade, the thickness and the strength of the material:
1) Softer metals take less. Soft aluminium and copper alloys are commonly listed well below steel, because they fracture at lower stress and roll over easily.
2) Mild steel sits in the middle. Many handbooks print 5 to 10 percent per side for shearing mild steel, and tool builders often keep a house number inside that band.
3) Harder grades take more. Industry guidance for advanced high strength steel rises from roughly 6 percent on mild steel to 16 percent and beyond as tensile strength climbs past 1400 MPa, which affects every cut in the die rather than one station.
Direction of application is where the two operations part company. Piercing adds the total clearance to the die opening, and blanking subtracts the total clearance from the punch. Grind the same figure into the same tool the wrong way round and the finished part misses nominal by twice the clearance, which on a 1.5 mm sheet at 10 percent per side is 0.30 mm of error before any other variation enters the picture.
Charts that publish separate columns for the two operations tend to give piercing the wider band, and the reason is worth spelling out. A pierced hole is usually the dimension a fastener, a shaft or a mating panel reads, and the punch that creates it is the same punch that wears. Loosening the clearance a little reduces punch wear, which keeps hole size more stable across the life of the tool. A blanked outline is often a handling edge, a seating edge or a trim line, so the balance there shifts toward edge quality and toward holding blank size on target.
Two failure modes frame the range. Clearance that is too small forces the fracture from the punch edge and the fracture from the die edge to miss each other, so the metal is cut twice along a secondary shear band. Cutting force rises, the punch is gripped on withdrawal, stripping force climbs, and slugs expand and jam in the die. Clearance that is too large lets the top surface roll over before shearing begins, thickens the burr, coarsens the fracture zone and loosens the dimensional spread. Both ends of that range cost money, and the middle is the cheap part.
Read the convention before you read the number. Total clearance is twice the per-side value, because the gap appears on both sides of the punch. A 1.5 mm sheet at 10 percent per side carries 0.15 mm at each edge and 0.30 mm across the diameter, so a 10.00 mm pierced hole needs a 10.30 mm die opening. If one side of the conversation is speaking per side and the other is speaking total, the tool is built with a gap that is either half or double what was intended, and the error is measured in tenths of a millimetre on a hole allowed a hundredth. Ask for the convention in writing, then ask for the die opening on one specific hole from the drawing. Two numbers that agree settle the question in seconds, and neither one can be argued about later.
The same trap appears when an existing tool is reviewed. Measure the punch, measure the die opening, subtract to find the total clearance, halve it, and divide by sheet thickness to express the result per side. A tool that measures 12 percent per side was probably designed that way, and one that measures 6 percent was probably designed as 6 percent.
Material condition belongs in the same conversation. Annealed, cold rolled and work hardened forms of one alloy sit in different parts of the recommended band, and a mill certificate showing strength at the top of its range shifts the starting point.
A stamped bracket usually carries three dimensions that have to agree with something else: the outer contour, the pierced holes, and the position of one relative to the other. Each behaves differently, and each is produced by a different cutting edge, so handing all three the same band makes a comfortable part unbuildable.
| 01Blanked outline. Carried by the die opening and worn larger over time. Treat it as a general tolerance unless it seats, seals or aligns. Where it does locate something, dimension that function from a hole instead of from the edge. | 02Pierced hole. Carried by the punch and worn smaller over time. This is the dimension a fastener reads, so it usually deserves the tightest band on the sheet and a one-sided limit that matches the direction of wear. |
| 03Hole position. Set by strip layout, piloting, feeding accuracy and how the part sits in the die, not by punch diameter. Position is normally the loosest of the three, and the one most often over-specified. | 04Mating part. Belongs in the stack even when it is bought elsewhere. A 0.05 mm hole tolerance against a 0.10 mm mating boss leaves nothing for the stamping house and everything for the assembly line. |
Take a 1.5 mm cold rolled bracket, 60 mm by 35 mm, with four 6 mm holes for M5 screws. Set the outline at plus or minus 0.20 mm, because nothing locates against it. Set hole diameter at 6.00 mm plus 0.08 mm and minus nothing, because the punch wears toward the small side and the screw only reads the low limit. Set hole position at plus or minus 0.10 mm from two holes used as a datum pair rather than from the blanked edge. That split leaves the outline free to drift with die wear, puts the tight band on the dimension a screw reads, and keeps position measured against features produced by the same class of cut.
Choosing the datum pair is the step most drawings skip. Dimensioning hole position from a blanked edge drags the behaviour of a second cutting edge, its wear direction and its inspection setup into one number. Nothing about the part changes, and the achievable position tolerance gets worse by roughly the distance the outline moves. Datum holes cut in one station, or in stations close together on the strip, keep that stack short.
Ronghai's published production figures are 0.05 mm as the standard tolerance and 0.02 mm on critical dimensions, with the actual requirement taken from the customer drawing. Those numbers work well for planning, and they also mark the point where a conversation should start rather than a default to fall back on. A 0.02 mm position tolerance on a 60 mm blank is a different project from the same callout on a 15 mm washer. Our notes on realistic stamping tolerances set the practical bands by feature and by grade.
Every sheared edge carries a signature. The punch presses the top surface down before shearing begins, which leaves a rounded rollover. A burnished band follows, where metal is compressed flat against the cutting edge. Fracture takes over from there, and the last metal to separate stretches outward as a burr on the exit face. Four zones, in that order, on every blank edge and every pierced hole.
| Rollover, punch entry | Burnish, smooth band | Fracture, rough angle | Burr, exit face |
Figure note. The burr sits on the side the metal leaves, and the rollover sits on the side the punch enters.
That sentence decides burr direction on any part, and it explains why direction can flip between two operations on the same sheet. In a line die or a progressive die where every punch travels downward, the blanked contour and the pierced holes both push metal out through the bottom, so rollover sits on the upper face and the burr sits on the lower face of both features. Nothing is reversed, and the part comes out consistent.
A compound die behaves differently, and this is where the familiar claim about opposing burrs comes from. Inside a compound die, the die block is mounted in the upper shoe with the piercing punches, while the blanking punch works from the lower die set and pushes the part upward. The two operations therefore cut in opposite directions, and the blank edge and the pierced hole end up with their burrs on opposite faces of the same part. The strip layout did not change, the part did not change, and the burr map changed completely.
Direction of every punch is fixed during tool design, which makes it one of the cheapest decisions to influence and one of the most expensive to reverse. Moving a piercing punch to the other shoe after the die exists means rebuilding the die set. Deciding the same thing during the DFM review costs a sentence in an email. A note on the drawing naming the face that may carry the burr converts a preference into a requirement, and a supplier reading it will place the punches accordingly.
A burr is small enough to ignore on a bench and thick enough to ruin a joint. Heights around a tenth of material thickness are normal for a healthy tool on mild steel, which on a 1.5 mm sheet means a burr approaching 0.15 mm. That is enough to hold a flange off a seating face or push a sliding fit out of clearance.
Four situations turn burr direction from a workshop detail into a drawing requirement:
1) A seating face. If a flange lands on the face that carries the burr, the joint closes on the burr instead of on metal, and every torque figure in the assembly instructions is measured against the wrong stack height.
2) A sliding or rotating interface. Burrs act as cutting edges against a mating surface, and a shaft running against a burred bore wears both parts.
3) A coated or plated part. Plating and coating build thickness over a burr as well as over base metal, and a burr on a critical face changes the finished dimension after the part has already passed stamping inspection.
4) Handling and sealing. Burrs cut gloves, cut gaskets and cut the operator reaching into a bin. Where a seal sits against a stamped edge, flatness of that edge belongs in the same conversation.
Deburring is the usual answer, and it is not free. Tumbling, grinding and polishing all appear on the secondary operation list for a reason, and each one adds handling, a process step and a new dimension to control. A part that will be tumbled anyway can carry a looser stamping band, because finishing removes the burr and normalises the edge. A part that ships straight off the press with only a coating has to have burr direction decided at the tool design stage, because nothing later in the route will fix it.
Direction is the useful callout, and height is the useful acceptance measure. Direction tells the tool designer which way each punch should travel, and it costs nothing at that stage. Height tells the inspector what to reject, and it belongs next to the burr note rather than buried in a general tolerance block. A number without a direction leaves the supplier free to place the burr on the face you needed clean, and a direction without a number gives the inspector nothing to measure.
Once both cuts are defined, the remaining question is how they are organised inside the tooling. Three arrangements cover most stamped work, and each one changes what a drawing change costs later.
| 01Single operation die. One cut per stroke, one operation per die. Cheapest to build and easiest to correct, with the part moved between dies by hand or by a transfer device. It suits prototypes, low volumes and large parts where a multi-station tool would be uneconomic. | 02Compound die. Blanking and piercing in one stroke, with internal and external features cut before the part leaves the station. Flat parts, washers and precision plates live here, and the arrangement brings higher dimensional accuracy because both cuts share one locating event. |
| 03Progressive die. The strip advances one pitch per stroke and stations pierce, notch, form and coin in sequence before the part is cut free at the end. Holes cut early stay round through later forming, which is the main reason the sequence is arranged that way. | 04Volume decides the choice. Low volumes lean toward a single operation die, medium volumes toward a compound die, and high volumes toward a progressive die, with automated progressive stamping at the top of the range. |
A compound die gives the outside edge and the holes one shared reference, because both are cut while the strip is held in the same position. A progressive die does not, and its accuracy depends on how well the strip is piloted as it advances from station to station. Neither arrangement wins in the abstract. One holds position on a flat part with no forming, and the other earns its price on a part with bends and drawn detail that would have to be added somewhere else otherwise.
Changing a sequence after the die exists is a rebuild rather than an adjustment, which is why the strip layout deserves a review of its own on any part with more than a few features. Features that must hold position belong in the same station or in adjacent stations, and features that only have to clear something can travel further down the strip. Customers reviewing a new bracket can send the drawing, the mating part and the assembly function together. Our DFM guidance for stamped parts covers the design side feature by feature, and this page covers the cutting operations themselves.
A worked example makes the difference between a buildable drawing and an expensive one. The part is the 1.5 mm bracket from earlier, with a 60 mm by 35 mm blanked outline and four pierced holes. Six lines carry the intent:
1) Outline, 60.00 mm and 35.00 mm, plus or minus 0.20 mm. General tolerance, because nothing locates against it and the die opening will wear larger over the life of the tool.
2) Holes, 6.00 mm plus 0.08 mm, minus zero. One-sided, because the punch wears toward the small side and the fastener only reads the low limit.
3) Position, plus or minus 0.10 mm from holes A and B as a datum pair. Datum features made by the same class of cut, so the position stack does not inherit outline wear.
4) Edge distance, 2.5 mm minimum from hole edge to blanked edge. Roughly one and a half times the thickness, which keeps the web strong enough to survive shearing without distorting.
5) Burr on the lower face, maximum 0.10 mm. Direction plus acceptance measure, placed next to the hole callout rather than in the general note block.
6) Material, cold rolled steel to the named grade, 1.5 mm nominal. Thickness variation and residual stress in the incoming coil both reach the sheared edge, so the certificate belongs in the file next to the inspection report.
Two of those six lines do most of the work. The one-sided hole tolerance tells the supplier which direction of wear is acceptable, and the datum pair tells the inspector which features to measure from. Take either one away and the same part becomes a negotiation instead of a specification. Remarkably little changes between a drawing that stamps comfortably and one that generates months of correspondence, and the difference usually sits in those two lines.
Whether a tolerance is achievable depends on material, thickness, tooling and process control together, and a modest looking position callout can turn aggressive once strip piloting and material variation join the stack.
A die that produces a perfect first article will not produce a perfect ten-thousandth part, and the drift is predictable rather than mysterious. Knowing which variable pushes which dimension turns a rejected lot into a short conversation about tool maintenance instead of a long one about capability.
Four causes account for most of the movement:
1) Punch wear closes the holes. Every stroke removes a little material from the cutting edge and the hole follows the punch down, which is the main reason a hole tolerance should be one-sided.
2) Die opening wear opens the outline. The blanked contour drifts the other way, so the part grows while the holes shrink, and a drawing dimensioning position from the outline carries both movements in one number.
3) Incoming material moves the whole result. Thickness variation, residual stress and coil set arrive with the strip, and a clearance calculated on nominal thickness now sits on a sheet that is not nominal.
4) Regrinding resets the clearance relationship. Sharpening a punch or re-cutting a die opening changes the physical gap, so a tool built at 10 percent per side may run tighter or looser afterwards.
Burr height is a wear indicator, not a quality guarantee. A long standing shop rule targets a burr below roughly ten percent of material thickness, and an increase past that threshold usually means the cutting edges need attention. On high strength grades the rule loses its power, because a low ductility material fractures before it can raise a tall burr and the edge can be badly worn while the burr still measures small. Read the burnish band and the fracture zone along with burr height, and treat the three together as the state of the tool.
Inspection practice reflects that reality. Burr height, hole diameter and hole position appear on in-process inspection sheets and are checked at startup, every fixed quantity, after a tool adjustment and after a material change. Triggers matter as much as items, since a measurement taken after new coil was loaded answers a different question from the same measurement taken mid-run, and that is where a buyer finds out whether the plan was followed.
Nothing on the list needs a statistical argument to resolve. A tool holding hole position within a hundredth of a millimetre on the first article while the burr climbs through the run is telling you about edge condition, and the useful response is a maintenance interval. Ronghai works to ISO 9001 and IATF 16949 as a general statement of the management system, with documentation to match.
The difference between a comfortable project and an expensive one usually shows up in the answers a supplier gives before tooling starts. Six questions cover most of the ground.
Ask before the quotation, not after the tooling order.
☐ 1) Which cutting edge carries each dimension on my part? The answer separates the features that wear one way from the features that wear the other, and it decides where the tight band belongs.
☐ 2) Is the clearance figure per side or total? Confirm it against the die opening for one specified hole, because that single number removes the most common tooling error in this family of work.
☐ 3) Which face will carry the burr, and what burr height is acceptable? A direction and a number agreed before the punches are placed, since neither one changes cheaply afterwards.
☐ 4) Does the part go into a compound die or a progressive die, and why that choice? The answer sets how position tolerance will be produced and how a design change will be priced later.
☐ 5) Which dimensions will be inspected, at what interval, and on which instrument? A first article report and a CMM report mean little if the part never sees them again during the run.
☐ 6) Which tolerances are functional, and which could open without hurting the assembly? Suppliers can usually read that from the drawing, and they rarely volunteer it.
It proves that the tool made one good part with a fresh cutting edge, which is the moment when hole size sits closest to nominal. The same tool will drift as the punch wears, so the first article belongs in a file alongside the inspection interval and the tool maintenance plan rather than standing alone as evidence of capability. A buyer reading a first article report on its own is reading the best case, and the number that matters for production is the one the process holds at the end of a run.
A supplier who can answer all six questions has thought about the part. One who answers the first two and defers the rest may still build a workable tool, and the risk then sits in whatever changes later. Precision work with tight hole position and tight hole diameter is usually won or lost on those answers, and the conversation is worth having on a part that looks simple.
A blanked outline and a pierced hole leave the same press stroke with the same four zones on their cut faces, and they behave differently for the rest of their lives. The die opening owns the outside size, the punch owns the hole, and wear pushes those two dimensions apart for as long as the tool runs. A burr lands on the face the metal leaves, which means its direction follows punch travel and can be inverted inside a compound die without anyone touching the drawing.
| Put the tolerance where the function is. The tightest band belongs on the dimension a fastener, a shaft or a seal reads, and it should be one-sided in the direction that matches tool wear. Everything that only has to clear something can take general tolerance and pay for it in nothing. | Settle the mechanics before the tooling. Clearance convention, burr direction and datum choice are three sentences at the quotation stage and three rebuilds afterwards. A drawing that states all three gets a more useful price, because the supplier can quote the process instead of an assumption. |
Most decisions on this page belong to the drawing rather than to the press. Whoever writes the callouts decides which dimension will be argued about in six months. Buyers comparing quotations on a pierced and blanked part can send the drawing along with the mating component and the assembly function, and the tooling discussion turns into a matter of confirming arithmetic. Ronghai produces precision metal stamping parts with pierced holes and blanked contours on the same tooling, and covers the multi-station route on the progressive die stamping capability page.
About the Manufacturer Behind These Pierced and Blanked Parts
Ronghai is a Chinese OEM metal stamping manufacturer producing progressive die, transfer die, compound die, deep drawn and precision sheet metal stamped components for buyers and engineers worldwide. ISO 9001 and IATF 16949 are held, and standard documentation includes material certificates, first article inspection reports, CMM reports and salt spray reports. Engineering review and DFM are completed before tooling design begins, so clearance, burr direction and datum questions are settled while changes are still free.
Related Stamped Parts Built From Blanked Contours and Pierced Holes
Typical output includes brackets, panels, enclosures, chassis parts, washers, terminals, contacts, busbars and mounting plates produced on carbon steel, stainless steel, aluminium, copper alloys, galvanized steel, HSLA and spring steel, from 0.3 mm to 20 mm thick. Send the 2D drawing, 3D model, material grade, annual quantity and the tolerances that will be inspected, and the reply covers process route, tooling approach and an inspection plan sized to your volume.
Inquiry
Article Navigation
About the Manufacturer Behind These Pierced and Blanked Parts
West side of Guangzhou North Road, Jiaozhou City, Qingdao City, Shandong Province
Copyright © 2025 Qingdao Ronghai Mould Products Co., Ltd. All Rights Reserved.
Powered by HiCheng
