Common Sheet Metal Fabrication Design Myths & Mistakes (And How to Avoid Them)

On paper, everything looks right.

The CAD model is clean, the dimensions line up, and the tolerances are clearly defined. Nothing appears to be out of place, yet when the part hits the shop floor, holes don’t align, bends don’t land where expected, or the finished assembly requires rework that was never part of the original plan.

For many teams, this is where frustration sets in. Nothing about the design raised red flags until the part actually had to be made. So why is fabrication turning out to be harder, slower, and more expensive than expected?

The answer is rarely a single mistake. More often, it’s a collection of incorrect assumptions about how sheet metal behaves, how tightly it can be controlled, and how features interact once material is bent, welded, and finished.

In this article, we break down the most common sheet metal fabrication mistakes and myths we see at Approved Sheet Metal. More importantly, we explain why they happen and how to catch them before production starts.

Myth #1: Sheet Metal Behaves Like Machined Plate

The biggest misconception we encounter is the assumption that sheet metal stays rigid and features remain exactly where they’re modeled. This makes sense if your background is in machining, where material is carved away from a solid block and geometry is controlled by cutting tools. But sheet metal fabrication is a fundamentally different process.

In sheet metal forming, the final location of features is harder to control than CAD models often suggest. As material is bent, it stretches and compresses, which affects how dimensions carry through the part. As a result, a hole that’s perfectly round in the flat pattern may come out slightly oblong after bending, and a dimension that looks exact in CAD may measure differently once the part is formed.

To the untrained eye, this might seem like a quality issue, but it’s simply how sheet metal behaves. A part can be made exactly as specified and still come back with features that don’t quite match what the designer expected. More often than not, the root cause is a design that didn’t account for material movement during forming.

Mistake #1: Unrealistic or Blanket Tight Tolerances

In machining, tight tolerances are standard. Values like ±0.002 inches are routine and achievable, so it’s easy for engineers trained in that environment to apply the same expectations to sheet metal design. Often, every dimension gets tightened “just to be safe.” It feels cautious, but in sheet metal fabrication, it usually creates more problems than it solves.

The core issue is tolerance stacking. In sheet metal fabrication, achievable tolerances depend on what is being dimensioned and how the part is formed. For example, dimensions taken from a formed edge to a hole or from a sheared edge to a bend can typically be held to around ±0.010 inches. Dimensions that carry across multiple bends introduce additional variation and are typically held to looser tolerances, such as ±0.015 inches across two bends, with greater variation across more complex formed features.

When those accumulated variations push a dimension outside the specified tolerance, it’s easy to assume there’s a workmanship problem. In reality, the issue often starts with drawings that call for tolerances tighter than the process can reliably hold in sheet metal fabrication. When that happens, the shop has to compensate. That can mean additional setups, manual measurement and adjustment, or secondary operations that were never part of the original quote. In some cases, the tolerance simply can’t be held consistently, and parts get rejected even though they would have functioned perfectly in the assembly.

Another common issue is applying tight tolerances across the entire drawing, including features that don’t actually require that level of precision. This forces unnecessary work on the whole part when only a few dimensions truly matter for fit or function.

A better approach is to be deliberate about where precision actually matters. Identify the dimensions that are critical to fit or function, and communicate that intent clearly to your fabricator. Then, relax tolerances everywhere else. In doing so, you get precision where it adds value and avoid unnecessary cost, rework, and lead time where it doesn’t.

Mistake #2: Features That Fight the Forming Process

One of the fastest ways to create problems in sheet metal fabrication is by adding features that don’t play well with the forming process. These designs often look reasonable in CAD, but once the material is cut and bent, small details can cause distortion, misalignment, or added complexity on the shop floor.

Holes Placed Too Close to Bends

One common example is placing holes or slots too close to a bend line. When sheet metal is bent, the surrounding material stretches and compresses, and features located too close to the bend can distort during forming. Approved Sheet Metal’s design guidance recommends placing holes at least three times the material thickness away from bends to help prevent this distortion. Keeping features a sensible distance from bends improves consistency and reduces surprises on the shop floor. When that spacing isn’t possible, it’s worth discussing alternatives early, such as relocating the feature or adjusting the forming sequence.

Tabs, Cutouts, and Short Flanges

Narrow tabs, closely spaced cutouts, and very short flanges can also create problems during forming. These features tend to flex or distort under bending forces, especially in thinner materials. Short flanges, in particular, can interfere with press brake tooling or require additional setups that weren’t originally planned.

Designing tabs with enough width to remain stable during forming makes a noticeable difference. As a general guideline, tabs that are proportioned relative to the material thickness tend to form more consistently than very narrow features. When flanges must be short, it’s important to confirm they’re compatible with available tooling early in the design process.

Sharp Internal Corners

Sharp internal corners are another detail that often causes problems in sheet metal fabrication, as they concentrate stress during forming and can complicate cutting and bending operations. Over time, those stress concentrations can also lead to cracking or reduced durability in the finished part.

Adding small internal radii helps parts form more predictably and distributes stress more evenly through the material. Even a modest radius can reduce forming issues and improve consistency without affecting function.

Quick Reference: Common Mistakes and Smarter Alternatives

Many sheet metal fabrication issues stem from reasonable design assumptions that don’t always translate cleanly to the shop floor. The table below summarizes the most common mistakes we see, along with design choices that help avoid unnecessary cost, rework, or delays.

Common Design Mistake	Why It Causes Problems	A Better DFM Approach
Applying tight tolerances to every dimension	Forces extra setups and higher cost without improving function	Identify critical dimensions and relax the rest
Designing sheet metal like machined plate	Ignores material stretching and compression during forming	Account for bends and material movement
Placing holes too close to bends	Bending distorts holes and affects fit	Keep features clear of bend areas or review placement early
Using sharp internal corners	Creates stress concentrations and complicates forming	Add small internal radii
Choosing material based only on strength or cost	Can crack, warp, or be difficult to form	Balance strength, formability, and environment
Assuming finishes hide imperfections	Coatings often highlight surface flaws	Define cosmetic requirements early
Ignoring coating thickness	Added buildup affects hole sizes and fits	Adjust tolerances to account for finishing
Skipping manufacturability review	Issues surface late, causing delays or scrap	Involve your fabricator early

Mistake #3: Treating Material Selection as a Checkbox

While material choice matters in any manufacturing process, it plays a more immediate role in sheet metal fabrication. Material selection directly affects whether a part can be formed cleanly, how it behaves during welding, and how reliably it performs once it’s in use.

Hard tempers are one of the more common pitfalls we see. Materials selected primarily for their strength often don’t have the ductility needed for bending, which can lead to cracking during forming. Aluminum is a good example. Engineers frequently specify 6061 because it’s the go-to choice in CNC machining, but 6061-T6 doesn’t tolerate forming well and can crack under relatively modest bend forces.

For sheet metal work, 5052 aluminum is usually a better fit. It’s commonly available in sheet form, more forgiving during bending, and far less likely to crack when forming tight radii, hems, or offsets.

Thickness introduces similar tradeoffs. Very thin stainless steel can be difficult to keep flat and may warp during welding. In many cases, increasing the thickness slightly makes the part easier to control and more predictable to fabricate.

At the same time, material strength plays a role. When rigidity is the goal, it’s sometimes possible to use thinner stainless steel instead of thicker mild steel, since stainless offers higher inherent strength.

The operating environment matters just as much. Mild steel used outdoors will rust without proper corrosion protection. Aluminum, while lightweight and corrosion-resistant, may not provide enough rigidity in high-stress structural applications. A material that looks fine on a spec sheet can fall short once the part is exposed to real-world conditions.

Mistake #4: Underestimating Finishing and Cosmetic Requirements

It’s easy to think of finishing as a cosmetic decision made at the end of a project. But finishes affect more than appearance. They influence fit, handling, and scheduling in ways that can create problems if they aren’t considered early.

Cosmetic Expectations

Because sheet metal shows handling, minor marks and scratches are a standard part of the cutting and forming process unless cosmetic requirements are explicitly defined. If appearance matters, it must be called out on the drawing. Without that guidance, parts may be functionally correct but not visually perfect.

Grain Direction

Brushed finishes have a visible grain direction. When multiple panels meet in an assembly, mismatched grain is immediately obvious. If the drawing doesn’t specify grain orientation, parts may arrive with patterns running in different directions. They’ll be technically correct, but visually inconsistent. For enclosures or other visible assemblies, grain direction should be specified on the drawing.

Coating Thickness and Fit

In addition to altering the appearance of a part, powder coating and paint add measurable thickness. A buildup of even a few thousandths of an inch at edges, corners, or cutouts can affect fit, especially when multiple coated surfaces come together. As a result, a hole sized precisely for a fastener may be too tight after coating, and mating surfaces may no longer align as expected.

It’s also common to assume coatings will hide surface imperfections. In practice, powder coat and paint tend to highlight flaws rather than cover them up. That’s why a slightly textured surface often results in a more consistent finished appearance than an overly smooth one.

Custom finishes add another variable. Specialty colors or non-standard coatings can extend project timelines significantly, sometimes by weeks rather than days. If finishing is likely to affect delivery dates, it should be considered early in the project.

What Happens When These Issues Aren’t Caught Early

When design issues surface after production has started, the impact escalates quickly. Parts already cut or formed may need to be reworked, scrapped, or remade from scratch, wasting material and pulling machine time away from scheduled work. When that happens, lead times slip, delivery dates move, and costs can increase.

Late changes also introduce compounding delays. New programming, updated drawings, fresh material procurement, and re-sequenced operations all take time, pushing downstream processes like finishing, assembly, and shipping off schedule. In some cases, rush fees are required to recover lost time.

The most difficult scenario is discovering tolerance issues after mating parts have already been machined. Once those components are complete, the sheet metal design can’t be adjusted to accommodate achievable tolerances, locking the project into specifications that may be impractical or impossible to hit.

This is why we often recommend a “sheet metal first” approach. Reviewing sheet metal designs before mating parts are machined gives you room to adjust tolerances and geometry while changes are still easy to make. Once parts are already in production, that flexibility disappears.

The One Thing That Prevents Most Sheet Metal Problems

If there’s a single theme that runs through all of these issues, it’s this: parts go more smoothly when they’re designed with fabrication in mind and reviewed early.

That doesn’t mean becoming a sheet metal expert. It means being clear about what actually matters for the part and communicating that up front, such as:

• Which dimensions are critical to fit or function, and which ones have flexibility
• How the part is intended to work within the assembly
• What conditions it will be exposed to once it’s in service

When fabricators understand that context, they can point out potential trouble spots before material is cut and recommend adjustments that make the part easier to build without changing how it’s supposed to perform.

Sheet Metal Design Without the Surprises

Every one of these sheet metal fabrication myths and mistakes is common and understandable-but it’s also avoidable. Most of them come down to assumptions that make sense in CAD but don’t always hold up once material is cut, bent, and finished.

At Approved Sheet Metal, we review drawings with an eye toward how parts will actually be made. We flag potential issues, talk through alternatives, and work with teams to adjust designs before production begins-when changes are still simple and inexpensive.

Most of these issues are easiest to fix before an RFQ is ever sent. The earlier fabrication is part of the conversation, the fewer problems tend to show up later. Contact us to get started.