These problems come up regularly in sheet metal fabrication for one simple reason: generic CAD values that look appropriate on the screen don’t match the realities of the fabrication floor. For example, while SOLIDWORKS defaults to a 0.100″ bend radius, our team at Approved Sheet Metal recommends a radius of 0.030″ for most sheet metal projects up to 0.125″ thick.
That single mismatch can throw off every flat pattern in a design and lead to unnecessary revisions, delays, scrap, and back-and-forth.
The solution isn’t more experience or memorization-it’s having the right information at your fingertips during design. We put together this guide with that goal in mind.
Table of Contents
- 1 Bends are Where Most Problems Start
- 2 Design Features That Create Fabrication Problems
- 3 Hardware Selection Is a Sheet Metal Design Decision
- 4 SOLIDWORKS and CAD Setup
- 5 Applying Machining Tolerances to Sheet Metal is a Costly Mistake
- 6 A 5-Step Process for Putting the Toolbox to Work
- 7 The Engineer’s Toolbox at a Glance
- 8 Better Parts Start with Early Collaboration
Bends are Where Most Problems Start
When was the last time you automatically selected a K-factor of 0.5 when designing sheet metal parts? It’s a common CAD default that rests on one big assumption: the neutral axis is exactly halfway through the material thickness. While this is realistic for very soft materials or parts with very large bend radii, we recommend a K-factor of 0.3-0.5 for most practical applications.
Because the right bend allowance depends entirely on your material, thickness, tooling, and press brake setup, it’s important to use values that match your material and your fabrication partner’s tooling, rather than relying on CAD defaults. If you’re unsure what values your fabricator uses, call them before you finalize the design. It’s a short conversation that can prevent a long revision cycle.
Our ideal bend radius is 0.030″ for consistent parts with solid structural integrity, and we hold tolerances of ±1 degree on most bend angles. Here’s a detail that surprises many engineers: only about 15% of sheet metal prototypes we see at ASM require a bend radius equal to the material thickness. Many engineers default to this assumption anyway, which can force specialty tooling and drive up both lead time and cost.
The Math Behind the Chart
Five formulas govern how material stretches and compresses during bending: K-factor, bend allowance, bend deduction, inside setback, and outside setback. We break each of them down in detail here.
At ASM, we use the bend deduction formula daily to compute the values in our bend gains chart. Unlike generic references, we built this chart from our actual tooling and process data. It covers aluminum, cold rolled steel, and stainless steel, with material-specific thickness, radius, setback, and die values.
Download the Bend Gains Chart Here
Design Features That Create Fabrication Problems
Beyond bend calculations, the placement and sizing of common design features directly affect whether a part forms cleanly or creates problems on the fabrication floor.
Feature Proximity to Bends
Features placed too close to bends are among the most common sources of fabrication problems beyond bend calculations themselves. When holes, slots, and cutouts are too close to bend lines, they distort during forming, causing misalignment and dimensional inaccuracies. As a rule of thumb, place holes and slots at least four times the material thickness from the outside edge.
The specific edge-distance rules depend on thickness:
- When the material thickness is ≤0.036″, the hole should be 0.062″ from the edge
- When the material thickness is >0.036″, the hole should be at least 0.125″ from the edge
The one exception? Slots close to bends are acceptable if you apply a kerf cut.
Other Features That Create Challenges
Features such as louvers, embossments, and small tabs often require additional tooling, and several other feature types have specific dimensional rules that affect manufacturability:
- Notch minimums must be at least the material’s thickness or 0.040″ – whichever is greater (and no longer than five times its width)
- Tab minimums must be at least two times the material thickness or 0.126″ – whichever is greater (and no longer than five times its width)
- Hem return lengths must be a minimum of four times the material thickness
- Offset height tolerances must be ±0.012″ from the top of sheet/top of form, with an ideal offset radius of 0.030″
You don’t need to memorize these specifications, but you should have them at your fingertips when you need them. Our Sheet Metal Design for Manufacturing eBook covers all of this and more, with visual examples of what to do (and what not to do) when designing each feature type.
Download the Sheet Metal Design for Manufacturing eBook Here
This ebook will help you get the part geometry right, but it’s not the only dimension that trips up experienced engineers. Hardware selection is another.
Hardware Selection Is a Sheet Metal Design Decision
Beyond hole sizing, other common hardware mistakes include:
- Incompatible material choices. Mixing steel fasteners with aluminum or stainless steel parts causes galvanic corrosion over time. Steel is also softer than stainless, which means knurls won’t grip the material properly, and hardware can fall out under pressure.
- Selecting the incorrect thread size or type. The wrong thread specification leads to misalignment, stripping, or poor fastening strength.
- Overlooking load requirements. Failing to account for load requirements can cause an assembly to fail under stress. Consider shear strength, pull-out resistance, and vibration exposure when selecting fasteners.
- Ignoring environmental conditions. Exposure to moisture, chemicals, and extreme temperatures can weaken certain materials. Stainless steel or coated hardware may be necessary for harsh conditions.
Engineers commonly default to steel hardware because it’s the cheapest and most widely available option. And while it works fine for steel parts or those going to powder coat or zinc plate, it doesn’t hold up in all applications.
It’s equally important to consider material thickness when selecting self-clinching hardware such as PEM nuts, studs, and standoffs, as these fasteners require specific sheet thicknesses to achieve full strength and proper installation.
We’ve created two downloadable references to help engineers get hardware right before drawings leave the desk. Our Hardware Hole Sizes Chart is a print-friendly resource for correct hole diameters by hardware type, and our Hardware Reference Sheet maps hardware compatibility across materials and finishes, including installation timing and minimum thickness requirements.
Download the Hardware Hole Sizes Chart HereDownload the Hardware Reference Sheet Here
Now that you have the resources to handle part geometry, feature rules, and hardware specifications, the next question is whether your CAD setup is actually reflecting them.
SOLIDWORKS and CAD Setup
There is no shortage of SOLIDWORKS training resources available for engineers designing machined parts. But when it comes to sheet metal design, equivalent resources are much harder to find. Most programs don’t cover how to set up a sheet metal model that translates cleanly to fabrication. That gap shows up in the files shops receive every day.
At ASM, our estimating and engineering team lives in SOLIDWORKS, while also understanding what happens when those files reach the press brake. That combination of deep CAD knowledge and hands-on fabrication experience is what shapes the design resources we’ve built.
Before we get to those resources, here are two quick tips:
-
Start in the sheet metal environment.
Design sheet metal parts using the sheet metal toolbar from the start rather than modeling a solid and converting it later. Converting can work, but it often creates cleanup issues when features don’t translate cleanly into sheet metal rules. Starting in the sheet metal environment helps SOLIDWORKS flag issues earlier-including problems with folding, unfolding, and flat pattern generation. -
Send both the formed model and the flat pattern.
Most quoting delays happen when a fabricator has to recreate a flat pattern or clarify missing assumptions about thickness, bend radius, or bend allowance behavior. Sending both upfront can significantly speed up your RFQ turnaround.
Here are a few other CAD-specific resources to help troubleshoot and streamline the part design process:
- From setting bend parameters to navigating common modeling questions, our SOLIDWORKS Tech Tip Videos offer practical, step-by-step guidance on how to design sheet metal parts for efficient fabrication.
- Our CAD Tooling Library provides pre-designed 3D tooling options that engineers can plug directly into their designs, eliminating the need to build basic sheet metal features from scratch. It’s a straightforward time-saver that ensures the features you’re designing are manufacturable from the start.
Whether you’re new to sheet metal design in SOLIDWORKS or you’ve been doing it for years, both resources are worth bookmarking. We update them regularly, and our SOLIDWORKS Sheet Metal Design Resources Page is the central hub where you’ll find everything in one place.
Access the Tech Tip Videos HereAccess the CAD Tooling Library Here
Applying Machining Tolerances to Sheet Metal is a Costly Mistake
Another area where design principles for machining are brought into sheet metal (with unintended consequences) is tolerancing. What seems like a perfectly normal tolerance by CNC machining standards can become a serious challenge on the fabrication floor. These tolerancing decisions may look minor in CAD, but they can lead to unnecessary secondary features or complex forming operations that significantly increase fabrication time and cost-without improving the quality or functionality of the part.
The key thing to understand is that achievable tolerances in sheet metal vary significantly depending on what’s being measured. A sheared edge to a hole is a very different proposition than a dimension across multiple bends. Applying one blanket tolerance across an entire part is one of the fastest ways to over-engineer a sheet metal design.
Here are ASM’s recommended default tolerances for precision sheet metal fabrication:
| Tolerance (in.) | Description |
|---|---|
| ± 0.005 | Sheared edge to hole |
| ± 0.005 | Two holes on one surface |
| ± 0.010 | Formed edge to hole |
| ± 0.010 | Sheared edge to bend |
| ± 0.015 | Across 2 bends |
| ± 0.030 | Holes across 2 bends |
| ± 0.030 | Holes across 4 bends |
| ± 0.030 | Formed part |
Note: These tolerances apply to parts within a 12″ envelope, measured in a restrained condition. Tighter tolerances are achievable depending on part geometry, but they come at a cost. Some dimensioning approaches, such as measuring holes across multiple bends or overall formed part dimensions, are not recommended where avoidable.
The range here tells the story. A feature on a single flat surface can be held to ±0.005″, but once bends are introduced, that tolerance opens up to ±0.030″, which is a sixfold difference. Designing with that reality in mind, rather than defaulting to the tightest tolerance available, is one of the simplest ways to reduce fabrication cost without sacrificing part performance.
Our Recommended Default Sheet Metal Tolerances reference sheet includes a visual diagram of a formed part with labeled dimension callouts corresponding to the table above. It’s a useful companion to keep alongside this article.
Download the Default Tolerances Reference Sheet Here
A 5-Step Process for Putting the Toolbox to Work
All of the resources in the Engineer’s Toolbox exist to solve the same problem: to help engineers close the gap between design intent and manufacturing reality for sheet metal parts. And while having them at the ready is an important first step, you must also know the right moment in the design process to put them to work.
-
Start with DFM rules.
Before you begin modeling, use the DFM ebook to validate basic geometry decisions such as thickness consistency, bend radius, hem/tab/notch sizing, and minimum edge distances for holes and slots. -
Set up CAD with real manufacturing assumptions.
Confirm that your material thickness, bend radius, and K-factor values in SOLIDWORKS match your fabricator’s actual process instead of the software’s default values. Start in the sheet metal toolbar so those settings are applied from the beginning. -
Check bend logic against real forming data.
Use the bend gains chart for validated values tied to actual tooling and materials. If your flat pattern dimensions don’t match what you expect, it’s usually a sign that your bend assumptions don’t match your fabricator’s process. -
Validate hardware against the sheet.
Confirm hole sizes, hardware type, minimum thickness requirements, and material compatibility before you finalize and release the drawing. -
Sanity-check tolerances.
Make sure your tolerances reflect a functional need, not habit. Use the tolerance reference sheet to confirm what’s realistic for the feature type you’re dimensioning.
The Engineer’s Toolbox at a Glance
| Resource | What It Helps With |
|---|---|
| Sheet Metal DFM eBook | Design rules for bends, hems, offsets, holes and slots, notches and tabs, countersinks, corners, and welding |
| Bend Gains Chart | Accurate flat pattern development based on material-specific thickness, radius, setback, and die data across aluminum, cold rolled steel, and stainless steel |
| Forming Tolerance Chart | Realistic dimensional expectations after bending, organized by feature type |
| Hardware Hole Sizes Chart | Correct hole diameters by hardware type |
| Hardware Reference Chart | Hardware selection based on material and finish |
When you’re ready to source materials and hardware, our Fabrication Industrial Suppliers page links to the suppliers we trust for hardware, industrial supplies, and raw materials.
Better Parts Start with Early Collaboration
The resources in this guide will help you design better sheet metal parts on your own. But some design decisions benefit from a second set of eyes-especially one with shop-floor experience.
When engineers bring ASM into the process early, our team reviews part geometry, materials, and forming requirements before production begins. That collaboration often results in small design adjustments that significantly improve manufacturability, reduce cost, shorten lead times, and prevent delays caused by redesigns.
This isn’t a service we reserve for customers. Whether you’re working with ASM or just looking for better design resources, we’re here to help. We built the Engineer’s Toolbox because we believe the best fabrication outcomes come from strong collaboration between engineers and manufacturers, regardless of who’s building the part.
Bookmark this page and keep these resources handy. Download them, print them, and tack them to the wall so they’re there when you need them. And if you have questions about a project or want early design input, our door is always open. Contact us or request a quote to get started.