- Key Takeaways
- What Are Sheet Metal Tolerances
- The Four Types of Sheet Metal Tolerances
- What Affects Sheet Metal Tolerances
- General Tolerance for Sheet Metal
- What Is Tolerance Stack-Up?
- Sheet Metal Thickness Tolerance and the Gauge Chart
- Sheet Metal Tolerance Chart by Material and Process
- Sheet Metal Tolerance by Process
- Bending Tolerance for Sheet Metal and the K-Factor
- FAQ
- Wrapping Up
Sheet metal tolerances are the allowable range a finished dimension can deviate from the drawing before the part no longer works. Typical values run from about ±0.005 in (±0.13 mm) on tight, laser-cut features to ±0.060 in (±1.5 mm) on looser ones, with the exact figure set by the material, thickness, and process. Bend angles usually hold ±0.5° to ±1°.
The reason they matter: no cut or bend ever hits the exact size on the drawing. You spec a 25mm edge. The finished part measures 25.04, or maybe 24.97. The tolerance is how far off you're willing to let that run before the part won't work. Too loose and it rattles around where it should sit. Too tight, and you're paying extra for accuracy that the part never needed.
Some of the gap is the metal itself. A sheet is never dead flat, and it's never one even thickness across its whole face, and that's true before a single machine touches it. The rest turns up during the work, since cutting, bending, and punching each drift inside their own range. Both stack up. Both need numbers wrapped around them.
That's really all a tolerance is. A set of limits that still count as a good part.
This guide runs through the four kinds of tolerance you'll see called out on drawings, the factors that quietly move them off target, the criteria behind standard sheet metal tolerances, and a full set of sheet metal tolerance charts with real figures for aluminum, stainless, and steel.
Key Takeaways
A tolerance tells the shop how far a finished dimension can wander from nominal before the part is scrap.
Material tolerance covers thickness and flatness. Fabrication tolerance covers the dimensions and angles made during cutting and forming.
Material type, tooling wear and the chosen process all shift tolerances, and thickness and flatness feel the raw stock the most.
Asking for tighter tolerances than the job needs burns money and lead time, so go tight only where function says you have to.
A fabricator who knows where each process gives and where it holds will help you shrink tolerance stack-up and land cleaner parts.
Table of Contents
- What Are Sheet Metal Tolerances
- The Four Types of Sheet Metal Tolerances
- What Affects Sheet Metal Tolerances
- General Tolerance for Sheet Metal and the Standards Behind It
- What Is Tolerance Stack-Up?
- Sheet Metal Thickness Tolerance and the Gauge Chart
- Sheet Metal Tolerance Chart by Material and Process
- Sheet Metal Tolerance by Process
- Bending Tolerance for Sheet Metal and the K-Factor
- FAQ
What Are Sheet Metal Tolerances
A tolerance is the room you leave between the dimension you drew and the dimension that shows up off the machine. Nobody hits a number dead on, every time, forever. So the tolerance draws the line that still passes as a good part. Spec it sensibly and parts mate without a fuss. Spec it badly, and you're staring at rework, rejects, or a quote that climbs for accuracy the part never needed.
Sheet metal sorts its tolerances into two camps.
- Material tolerances describe the raw stock before any fabrication starts. Two matter most. Thickness, the allowed swing in how thick the sheet is, and flatness, how far the surface strays from truly flat. This variation gets baked in at the mill, so it's already sitting there before the first cut.
- Fabrication tolerances describe what happens once the sheet is on the machine. Dimensional tolerance covers size and where features land, things like length, width and hole position. Angular tolerance covers how close a bend or a weld sits to the angle you asked for.
Keep those four straight, and the rest of this stops feeling slippery.
The Four Types of Sheet Metal Tolerances
#1 Dimensional Tolerances
Dimensional tolerances carry most of the drawing. Length, width, diameter, where the holes sit. These are the numbers that decide whether two parts actually meet when they're supposed to. If you dial them in, and everything will slot together. Leave them loose, or worse, contradicting each other across the print, and you end up with gaps, parts that sit proud of where they should, and a trip back to the floor to do it again.
Most shops don't make up their own numbers for this. They reach for a published standard. ISO 2768 and ASME Y14.5 each lay out how to apply a general tolerance for sheet metal dimensions, and that shared language is what keeps the designer and the fabricator on the same page instead of arguing after the fact.
On custom work the pattern tends to repeat itself. Tight on the handful of features that mate with something else, fairly loose everywhere the fit doesn't matter.
#2 Angular Tolerances
Angular tolerances set how far a bend or a weld can wander off its target angle before it's a problem. Where they really matter is on brackets, enclosures, and frames. Anything where the geometry stacks up bend on bend, which is mainly because one angle that's slightly off at the start throws everything downstream out of line with it.
Say a bend lands a degree off. That might show up as a sloppy fit, or stress loading a corner it was never meant to, or a part that simply won't go together. Most angular tolerances live in the plus or minus 0.5 to plus or minus 1 degree range. The right number for your part, though, shifts with what it's for, what it's made of, and how it gets formed.
Electronics is the demanding end of this. Parts jammed into tight housings leave no room to be casual about angles. Structural work is the opposite, and a looser call is usually fine. CNC bending buys you tighter angles since the press brake hits the same stroke over and over with hardly any drift from one part to the next. Then there's springback. Soft alloys pretty much stay put where you bend them. Higher strength steels behave differently, they kick back the second the punch lifts, so you overbend a touch to let them spring home to square.
#3 Thickness Tolerances
Now the raw material gets a say in things. Every sheet turns up with a thickness spread already in straight from the mill. Pull two sheets from one batch and they won't match exactly. Jump between batches and the gap widens. Even a single sheet drifts in thickness from its edge in toward the middle. All of that traces back to rolling, hot and cold both, the process that flattens a slab down into usable sheet.
On plenty of parts a small swing in thickness just doesn't matter. It's there, but it changes nothing you'd ever measure. Stack-ups are the exception. So are tight clearance assemblies. That's where the thickness you didn't account for shows up as load sitting unevenly, or a feature that wanders a hair out of place, then another, until the thing no longer lines up the way the print promised.
The two common stock types don't behave the same.
Hot rolled steel gets worked hot, north of roughly 1,700°F or 927°C, which makes it easy to shape. It comes off rough, softer and more giving, so it suits structural work, welding and general fabrication where exact size isn't the point. Cooling at room temperature with little grip on final size, it shows the widest thickness variation of the bunch.
Cold rolled steel is hot rolled steel pushed further at room temperature to sharpen its strength, its finish and its dimensional accuracy. Work hardening leaves it harder, stronger and smoother. It holds a far tighter thickness tolerance, which is why it lands in parts that have to hit their numbers.
Stand them side by side, and cold rolled takes strength, hardness, wear resistance and tightness, making it the pick for high-stress, accurate work. Hot rolled takes cost and forms or welds without complaint, so it belongs in heavy structures where surface finish and tight tolerance matter less.
#4 Flatness Tolerances
Flatness tolerance sets a limit on how far a surface is allowed to bow away from flat. On a small bracket you'll never think about it. Think panels, doors, enclosures. Warp sneaks in from a few directions, stress trapped inside the metal to begin with, the heat and pressure of cutting and forming, and honestly just getting knocked around on the shop floor. A panel with even a slight bow can seal poorly, rock under load, or read as cheap on an otherwise clean product.
Pulling a part back to flat costs you steps. Straightening. Leveling. Stress relieving, if it comes to that. Thin sheets are the ones that warp easy under the work. Thick sheets do the opposite, they sit on residual stress from the rolling line and then spring out of flat the second you cut into them and let it loose.
This is worth catching early, before the run is deep. It saves a pile of time and money, and it earns its keep in HVAC and electronics especially, where a flat face isn't a nice-to-have, it's on the spec.
What Affects Sheet Metal Tolerances
Plenty pushes tolerances around. It shakes out differently across the four types.
Dimensional tolerances move with material consistency, since a swing in thickness or hardness changes how a part cuts and forms. Tooling counts too, because worn punches and dies drift off target. Small variations in a multi part assembly can pile into real misalignment, an effect we call tolerance stack-up. Method matters as well, with laser cutting and CNC machining holding tighter than manual cutting or stamping. Heat off a plasma or laser torch can expand or shrink the metal and nudge the final size.
Angular tolerances ride on the material. Ductility and elasticity drive springback in the bend, and softer stock tends to wander further. Smaller bend radii are harder to repeat and often want special tooling. Press brake setup and die alignment feed straight into the result. Parts with a string of bends collect angle error along the way. Manual bending leans on the operator, so skill adds or trims the spread.
Thickness tolerances trace back to the stock. Hot rolled shows wider swings from its loose cooling. Cold rolled holds tighter from its finishing pass. The rolling process, the mill setup and the cooling rate all leave fingerprints. Stacked assemblies turn any thickness spread into misalignment, and parts after a polished finish usually favor cold rolled for its steadier thickness and smoother face.
Flatness tolerances suffer from batch to batch swings in raw stock and from within sheet variation like uneven rolling or trapped stress. Cutting that adds localized heat, laser and plasma, brings thermal distortion. Stamping and punching plant stress that can warp the sheet. Big or oddly shaped parts warp more where they go unsupported. Rolling, pressing, and stress relieving after the fact pull parts back toward flat, and cold rolled stock tends to hold flatness better thanks to its refined rolling.
General Tolerance for Sheet Metal and the Standards Behind It
Two standards do most of the work on a drawing.
ISO 2768 sets the general tolerance for sheet metal across linear and angular dimensions whenever a feature carries no callout of its own, sorted into classes from fine to coarse.
ASME Y14.5 runs the GD&T side, the language for form, orientation and position. Name one in the title block and you've told the shop how to read every dimension that doesn't carry its own number. If you lean on a published general tolerance for sheet metal, you're spared marking up every edge by hand.
What Is Tolerance Stack-Up?
Tolerance stack-up is what you get when a pile of small allowed variations add together across a part or an assembly. One bend can sit dead inside spec. Drop a critical hole on the far side of four bends, though, and the allowed error at each step lands on top of the last, so a feature that looked tidy on the model drifts well past where you meant it. This is the quiet reason so many parts fail inspection even when every single callout looked fair on its own.
The fix is mostly layout. Keep critical features on one flat plane where laser accuracy carries clean through, instead of spreading them over a run of bends. Pull dimensions from a single datum rather than chaining them nose to tail. And lean on a fabricator who'll flag a nasty stack-up before the part is cut, since catching it on the drawing costs a fraction of catching it at inspection.
Sheet Metal Thickness Tolerance and the Gauge Chart
Before you can talk sheet metal thickness tolerance with any confidence, you've got to know what your gauge number actually means in real units.
Gauge is a nominal call. A 16 gauge sheet of steel and a 16 gauge sheet of aluminum are not the same thickness, and the stock you get still varies inside the mill's own band. Measure a fresh sheet with a micrometer and you'll often read a few thousandths under the label, which is exactly why a tight sheet metal thickness tolerance can drift before a single bend happens.
Gauge to Decimal Reference
Here's a gauge to decimal reference for the materials that come up most. Values are in inches, with millimeters alongside for the steel column.
| Gauge | Steel (in) | Steel (mm) | Stainless Steel (in) | Aluminum (in) |
|---|---|---|---|---|
| 7 | 0.1793 | 4.55 | 0.1875 | 0.1443 |
| 8 | 0.1644 | 4.18 | 0.1719 | 0.1285 |
| 10 | 0.1345 | 3.42 | 0.1406 | 0.1019 |
| 11 | 0.1196 | 3.04 | 0.1250 | 0.0907 |
| 12 | 0.1046 | 2.66 | 0.1094 | 0.0808 |
| 14 | 0.0747 | 1.90 | 0.0781 | 0.0641 |
| 16 | 0.0598 | 1.52 | 0.0625 | 0.0508 |
| 18 | 0.0478 | 1.21 | 0.0500 | 0.0403 |
| 20 | 0.0359 | 0.91 | 0.0375 | 0.0320 |
| 22 | 0.0299 | 0.76 | 0.0313 | 0.0253 |
| 24 | 0.0239 | 0.61 | 0.0250 | 0.0201 |
Galvanized steel reads a touch thicker than bare steel at the same gauge, since the zinc coating adds to it. A good habit on a drawing is to call the gauge and the decimal together, something like 16 ga (0.0598 in), with the decimal noted as reference so nobody tries to hold a four place number on stock the mill never promised. If you manage to match the gauge to the job, you keep your sheet metal thickness tolerance realistic instead of fighting the material.
Sheet Metal Tolerance Chart by Material and Process
Hard numbers save you a lot of back and forth, so here is a sheet metal tolerance chart set covering the cutting and forming ranges plus thickness bands for the common materials. Treat these as your reference for standard sheet metal tolerances, then tighten only the features that genuinely need it.
Sheet Metal Tolerances, Laser Cutting and Bending
As a baseline, standard laser cutting and bending holds linear dimensions to ±0.45 mm and hole diameters to ±0.12 mm, tightening to ±0.20 mm and ±0.08 mm on precision work - with bend angles at ±1.0° standard or ±0.5° precision.
| Feature | Standard Tolerance | Precision Tolerance |
|---|---|---|
| Linear (X.XX) | ±0.45 mm | ±0.20 mm |
| Hole diameter | ±0.12 mm | ±0.08 mm |
| Angular | ±1.0 degree | ±0.5 degree |
| XYZ | ±0.45 mm | ±0.20 mm |
Material Thickness Bands, Standard Tolerances
Material thickness bands for standard tolerances run like this.
| Thickness Range | Standard Tolerance |
|---|---|
| 0.5 mm to 2.0 mm | ±0.05 mm |
| 2.0 mm to 5.0 mm | ±0.10 mm |
| 5.0 mm to 10.0 mm | ±0.25 mm |
| 10.0 mm to 20.0 mm | ±0.50 mm |
Aluminum Sheet Thickness Tolerance Chart
| Thickness (mm) | Sheet Width < 1000 mm | Sheet Width 1000–1250 mm |
|---|---|---|
| >0.40 to 0.50 | ±0.03 | ±0.04 |
| >0.50 to 0.60 | ±0.03 | ±0.05 |
| >0.60 to 0.80 | ±0.03 | ±0.06 |
| >0.80 to 1.00 | ±0.04 | ±0.06 |
| >1.00 to 1.20 | ±0.04 | ±0.07 |
| >1.20 to 1.50 | ±0.05 | ±0.09 |
| >1.50 to 1.80 | ±0.06 | ±0.10 |
| >1.80 to 2.00 | ±0.06 | ±0.11 |
| >2.00 to 2.50 | ±0.07 | ±0.12 |
| >2.50 to 3.00 | ±0.08 | ±0.13 |
| >3.00 to 3.50 | ±0.10 | ±0.15 |
| >3.50 to 4.00 | ±0.15 | ±0.18 |
| >4.00 to 5.00 | ±0.18 | ±0.22 |
| >5.00 to 6.00 | ±0.20 | ±0.24 |
Stainless Steel Thickness Tolerance Chart
| Thickness (mm) | Sheet Width < 1250 mm | Sheet Width 1250–2500 mm |
|---|---|---|
| 0.10 to <0.20 | ±0.01 | ±0.015 |
| 0.20 to <0.30 | ±0.015 | ±0.020 |
| 0.30 to <0.40 | ±0.020 | ±0.025 |
| 0.40 to <0.60 | ±0.025 | ±0.030 |
| 0.60 to <1.00 | ±0.030 | ±0.035 |
| 1.00 to <1.50 | ±0.035 | ±0.040 |
| 1.50 to <2.00 | ±0.040 | ±0.050 |
| 2.00 to <2.50 | ±0.050 | ±0.060 |
| 2.50 to 3.00 | ±0.060 | ±0.070 |
Q235 Carbon Steel Thickness Tolerance Chart
| Thickness (mm) | Sheet Width 600–1200 mm | Sheet Width 1200–1500 mm |
|---|---|---|
| <1.50 | ±0.17 | ±0.19 |
| >1.50 to 2.00 | ±0.19 | ±0.21 |
| >2.00 to 2.50 | ±0.20 | ±0.23 |
| >2.50 to 3.00 | ±0.22 | ±0.24 |
| >3.00 to 4.00 | ±0.24 | ±0.26 |
| >4.00 to 5.00 | ±0.26 | ±0.29 |
| >5.00 to 6.00 | ±0.29 | ±0.31 |
| >6.00 to 8.00 | ±0.32 | ±0.33 |
| >8.00 to 10.00 | ±0.35 | ±0.36 |
| >10.00 to 12.50 | ±0.39 | ±0.40 |
| >12.50 to 15.00 | ±0.41 | ±0.42 |
| >15.00 to 25.40 | ±0.44 | ±0.46 |
SPCC Cold Rolled Steel Thickness Tolerance Chart
| Thickness (mm) | Sheet Width < 1000 mm | Sheet Width 1000–1250 mm |
|---|---|---|
| <0.60 | ±0.05 | ±0.06 |
| 0.60 to 0.80 | ±0.06 | ±0.07 |
| 0.80 to 1.00 | ±0.07 | ±0.08 |
| 1.00 to 1.20 | ±0.08 | ±0.09 |
| 1.20 to 1.50 | ±0.09 | ±0.10 |
| 1.50 to 2.00 | ±0.10 | ±0.11 |
| 2.00 to 2.50 | ±0.12 | ±0.13 |
| 2.50 to 3.00 | ±0.13 | ±0.14 |
| 3.00 to 4.00 | ±0.15 | ±0.16 |
| 4.00 to 5.00 | ±0.18 | ±0.19 |
| 5.00 to 6.00 | ±0.20 | ±0.22 |
Sheet Metal Tolerance by Process
Different methods sit in different accuracy bands, so the process you pick quietly caps how tight you can spec in the first place. Here's how the common ones stack up side by side, and you can see Komacut's own machine tolerances for reference.
| Process | Linear Tolerance | Hole Tolerance | Angular Tolerance | Best Applied To |
|---|---|---|---|---|
| Laser cutting | ±0.005 to ±0.015 in | ±0.005 in | n/a | Thin to medium sheet, tight outlines |
| Waterjet cutting | ±0.005 to ±0.020 in | ±0.010 in | n/a | Thick stock, heat sensitive metals |
| Plasma cutting | ±0.030 to ±0.060 in | ±0.030 in | n/a | Heavy plate, less fussy work |
| CNC press brake bending | grows with flange length | n/a | ±0.5 to ±1 degree | Formed flanges, brackets, enclosures |
| Punching and stamping | ±0.010 to ±0.020 in | ±0.010 in | n/a | High volume runs of the same part |
These are typical industry ranges — actual capability varies with machine, material, and setup.
Laser cutting is about as accurate as it gets here. It'll reach as tight as ±0.005 inches on thin stock, though ±0.010 to ±0.015 inches is the day to day reality. Waterjet runs a similar band, give or take ±0.005 to ±0.020 inches, with no heat affected zone to fret over. Plasma sits wider, somewhere around ±0.030 to ±0.060 inches, which suits the heavier, less fussy jobs just fine.
Forming piles more variables on top of the cut. K-factor, springback, the way the bend deforms as it goes, they all feed the final number, and every extra bend angle widens the spread you've got to plan for.
Sheet Metal Stamping Tolerances
Stamping plays by different rules than cutting or bending. The die does the work here, and once it's cut, that die stamps out the same shape over and over, thousands of hits deep, barely wandering off the mark. So your parts come out near identical. That's the upside.
The cost of it lives in the tooling. A hardened die is a serious spend before you've made a single good part, and it only ever makes the one shape you cut it for. That's the whole reason stamping suits a long run and makes no sense for a couple of parts.
At volume, on tight features, sheet metal stamping tolerances will usually out-hold what you'd get off a press brake, and deep drawing takes it further still. The tooling bill only pays for itself once enough parts share it. Need ten pieces? Laser and bending win on cost, easily. So the real question with sheet metal stamping tolerances comes down to quantity. Make enough parts off that die and it earns its place. If you fall short of that number, it never does.
Bending Tolerance for Sheet Metal and the K-Factor
Bending is where tolerance gets hardest to pin down, since the metal stretches and shifts as it forms. The number that sits underneath all of it is the K-factor, and getting a handle on it is most of the job with bending tolerance.
Think of the sheet lying flat. Somewhere through the middle of its thickness runs the neutral axis, the layer that's neither getting stretched nor squashed. Bend the sheet, and that layer doesn't hold still. It slides toward the inside face of the bend.
What the K-factor does is put a number on that slide. Take where the neutral axis ends up, divide it by the full thickness of the material, and there's your value, K = t/MT. Real-world numbers sit between 0.3 and 0.5 for most metals. Textbooks reach for 0.446 out of habit. On the shop floor, 0.33 is a sensible place to start a general job and adjust from there.
Once you've got a K-factor, you can work out the bend allowance, the actual length of material the bend eats up. The formula reads BA = (pi / 180) × bend angle × (inside radius + K × thickness). Pair that with bend deduction, the amount your flat blank comes up short against the summed outside flanges, and you can lay out a flat pattern that forms into the part you drew rather than one running long at the flanges.
Some rough starting values are below. None of these are settled numbers, so lean on them as a first guess and expect to move off them. Your punch radius shifts the real figure. So does the width of your V-die. Whether you're air bending or bottoming changes it again, and even the direction of the grain in the sheet has a say.
K-Factor Starting Values
| Material | K-Factor Range |
|---|---|
| Mild steel | 0.40 to 0.45 |
| Stainless steel | 0.45 |
| Aluminum | 0.33 to 0.40 |
The best thing you can do is test it yourself. Grab a coupon, bend it in the tooling you'll actually run, measure what comes out, and work the K-factor backward from there. Skip that and trust a generic chart, and your first article might come back with flanges running a hair long, or a hair short.
Do it on real metal instead, and the bending tolerance for sheet metal comes in tight, and a tight part is one that drops into the assembly and stays there rather than looping back for rework. That one habit will do more for a clean flat pattern than any amount of leaning on the press brake.
Instant DFM Checking
Try Komacut's instant quotation tool
Get fast, accurate cost estimates that factor in material and fabrication tolerances, so you can plan, budget, and refine your sheet metal parts with confidence.
FAQ
What are the standard sheet metal tolerances?
Standard sheet metal tolerances usually run from around ±0.005 inches on tight features down to ±0.060 inches on the loose ones, and the exact figure tracks the material, the thickness and the process. Plenty of shops fall back on ISO 2768 or ASME Y14.5 as the baseline whenever a feature has no callout of its own.
What is the tightest tolerance you can hold in sheet metal?
On a single flat face, laser cutting will get you close to ±0.005 inches on thin stock. Add bends and that loosens off, since every formed feature brings its own variation and the part flexes while it's being worked.
Why are sheet metal tolerances looser than machining tolerances?
Machining carves features out of a solid block with one tool, so each one lands on its own terms. Sheet metal starts from stock that already varies in thickness, then gets cut, bent and stretched across a handful of machines, each with its own range. That mix makes formed parts a tougher ask to hold to machining grade numbers.
What is tolerance stack-up?
Tolerance stack-up is the sum of a lot of small allowed variations across a part or assembly. Spread critical features over several bends and the error at each step adds onto the last, which can shove a feature past where you wanted it even when every callout was fine on its own.
Which standard covers sheet metal tolerances?
Two do most of the work, and they cover different ground. ISO 2768 is the one for general linear and angular dimensions, sorted into classes that run from fine all the way out to coarse. ASME Y14.5 is a different beast, it's the GD&T standard, so it deals in form, orientation and position. Whichever one applies gets named up in the title block of the drawing. From there it quietly sets the tolerance on every dimension nobody called out by hand.
What is the K-factor in sheet metal bending?
The K-factor is the ratio of the neutral axis location to the material thickness, written K = t/MT. It usually sits between 0.3 and 0.5, and you feed it into the bend allowance to lay out a flat pattern that forms into the right size.
Does sheet metal gauge equal exact thickness?
No. Gauge is a nominal call, and the same gauge number gives a different thickness in steel, stainless and aluminum. Real stock also varies inside the mill's band, so check a gauge chart for the decimal and treat your sheet metal thickness tolerance from there.
How tight are sheet metal stamping tolerances?
Once the die is built, sheet metal stamping tolerances are excellent and repeat part to part with little drift, often beating press brake bending on tight features. The tradeoff is tooling cost, which is why stamping pays off on high volume runs rather than small batches.
Wrapping Up
Sheet metal tolerances really come down to four moving parts working together, dimensional, angular, thickness, and flatness, each one shaped by the material you pick, how the part gets fabricated, and what's going on around it on the floor.
The process you choose, laser cutting and CNC bending at one end, stamping and rolling at the other, sets the accuracy you can honestly hold. Parts that need genuinely tight numbers might call for stamping or deep drawing, while CNC bending and laser cutting suit the less sensitive stuff thanks to low tooling cost and short lead times.
Only chase tight numbers where the part genuinely needs them. Try to keep your important features off the end of a long chain of bends where the error piles up. And find a fabricator who'll spot a stack-up on the drawing, before anyone's cut metal. If you get those three right, the parts that come back will fit exactly the way your drawing said they would.