Countless products use sheet metal fabrication, from brackets and enclosures in the automotive and consumer electronics industries. There are a few avoidable design traps that can lead to project failures, delays, and additional costs. To avoid these mistakes, follow the tips in this blog post.
We’ll discuss the following missteps from material selection to fastener placement and finishing decisions:
- What is the mistake, and why does it happen?
- Real-world consequences.
- Numerical guidelines and formulas.
- Actional best practices.
Whether you’re a seasoned pro or new to sheet metal, these insights will help you design parts that are manufacturable and cost-effective.
Material Selection
What is the mistake, and why does it happen?
Choosing the wrong alloy or material thickness. Ignoring the key properties, such as ductility, tensile strength, or corrosion resistance. Failure to consider cost and availability.
Designers may default to familiar materials, overlook environmental factors, or fail to match the material properties to the application needs.
What are some real-world consequences?
- Cracking during forming, for example, using 6061-T6 aluminum for tight bends.
- Rapid corrosion, for example, occurs when using mild steels for outdoor applications without coatings.
- Overly heavy or expensive parts.
- Supply chain delays due to rare or hard-to-source alloys.
Guidelines and Numbers
| Material | Strength and Ductility | Corrosion Resistance | Formability | Cost |
|---|---|---|---|---|
|
Mild Steel |
Moderate |
Low (Needs Coating) |
Good |
Low |
|
304 Stainless |
High |
Good |
Moderate |
Moderate |
|
316 Stainless |
High |
Excellent |
Moderate |
High |
|
5052 Aluminum |
Moderate (Very Ductile) |
Excellent |
Excellent |
Moderate |
|
6061 Aluminum |
High (Less Ductile) |
Good |
Poor (T6 Temper) |
Moderate |
|
Copper |
Low Strength and Very Ductile |
Good |
Excellent |
High |
What are the best practices?
- Match the alloy to the application, for example, use 5052 aluminum for tight bends and 316 steel for marine environments.
- Double-check the ductility and formability of the material, and avoid choosing brittle alloys for complex shapes.
- There must be a balance between cost and performance. Don’t over-specify. Use the lowest-cost material that meets the requirements.
- Consult suppliers. Stick to standard gauges and available alloys.
- Talk with our team early in the design process. If you have questions about manufacturability and finishing compatibility, Prototek can give you feedback.
Specify Improper or Too-Tight Tolerances
What is the mistake, and why does it happen?
Applying machining-level tolerances, such as ±0.005 in to sheet metal, ignoring cumulative tolerances across bends, or failing to reference industry standards is a mistake.
The desire for precision, lack of familiarity with sheet metal processes, or copying tolerances from machined components.
What are some real-world consequences?
- Tighter tolerances can increase the scrap rates and costs.
- Parts may not fit together due to tolerance stack-ups.
- Delays may happen if excessive inspection and rework are required.
Guidelines and Numbers
- One-Surface Tolerance: ±0.005 in or 0.13 mm
- Across 3+ Bends: ±0.030 in or 0.76 mm
- Bend Angle Tolerance: ±1°
- Industry Standards: ISO 2768-mk and ASME Y14.5
What are the best Practices?
- Use standard tolerances. Only tighten them where functionality is necessary for critical pieces.
- Reference ISO 2768 or ASME Y14.5. These tolerances will be consistent, industry-acceptable tolerances.
- Account for cumulative errors. Loosen tolerances across multiple bends or large parts for the best results.
- Communicate critical features with the fabricating team. Clearly mark the features that require special attention.
Ignoring Minimum Bend Radius Guidelines
What is the mistake, and why does it happen?
If a bend radius is too small for the material, it will lead to cracking, thinking, or failed bends.
Not all materials behave the same. Don’t assume they will. Consult the material-specific data.
What are some real-world consequences?
- Bend radii that are too small can lead to cracks and fractures at the bend.
- They also cause excessive thinning, which can lead to the part weakening.
- Minuscule bend radii can lead to increased scrap and rework.
Guidelines and Numbers
These numbers are based on the minimum bend radius as a multiple of thickness (T).
- Mild Steel: 0.8T
- Aluminum Alloys: 2T
- Stainless Steel: 1.5T
- Note: A 0.030 in or 0.76 mm internal radius works for about 95% of cases.
What are the best practices?
- Materials have specific minimum bend radii, and understanding these will help you feel more competent in your design choices. For example, larger radii are recommended for brittle alloys like 6061-T6 aluminum, reducing the risk of cracks and rework.
- Use consistent radii across the part. Doing this will minimize tooling changes.
- Referring to material data sheets or conducting test bends ensures accurate bend radius application, reducing scrap and rework in critical applications.
Account for the bend allowance and the k-factor
What is the mistake, and why does it happen?
Don’t ignore the extra material needed to create bends, or use the wrong K-factor values. These can result in flat patterns that don’t yield the correct finished dimensions.
A lack of understanding of the bend mechanics, or default values without an adjustment for the material or process.
What are some real-world consequences?
- Parts will be too long or too short after bending.
- There may be assembly issues due to misaligned features.
Guidelines and Numbers
- Bend Allowance (BA) Formula: BA = (π/180) x Angle x (R + K x T)
- Angle: Bend angle in degrees.
- R: Inside bend radius.
- T: Material thickness.
- K: K-factor
- K-Factor Ranges:
- Air Bending: ~0.33
- Bottom Bending: ~0.42
- Harder Materials: Up to 0.5
What are the best practices?
- Don’t rely on defaults. Make sure to calculate the bend allowance for each bend.
- Adjust for material and bending methods, using the correct k-factor.
- Leverage CAD tools, many of which have built-in bend tables and calculators.
- For new materials or critical parts, test and validate the bends.
Poor Hole and Slot Placement
What is the mistake, and why does it happen?
Placing holes or slots that are too close to the edges or bends is a mistake. Making them too small for the material thickness is also a mistake.
These mistakes can happen when trying to maximize the space and a lack of awareness of constraints in fabrication.
What are some real-world consequences?
- These mistakes can lead to tearing or distortion during punching or bending.
- They can cause tool breakage or poor cut quality.
- Weak joints or failed features are another side-effect.
Guidelines and Numbers
| Feature | Minimum Dimension/Ratio |
|---|---|
|
Hole Diameter (Ductile) |
≥ 1.2x Material Thickness |
|
Hole Diameter (High Strength) |
≥ 2x Material Thickness |
|
Hole/Slot to Edge |
≥ 2x Material Thickness |
|
Hole/Slot to Bend |
Content |
What are the best practices?
- Follow the minimums, for example, use at least 1.2T for holes in ductile materials and 2T for strength.
- Don’t put holes too close to the edges or the bends. Make sure they are 2T from the edge, and follow bend-specific guidelines.
- For material-specific recommendations, consult fabrication tables.
- Especially for tabs and slots, test fit production runs.
Designing Inadequate Flange Lengths
What is the mistake, and why does it happen?
Flanges that are too short may lead to improper forming and can cause deformation or incomplete bends.
Not understanding press brake constraints or trying to save material or space can induce this mistake.
What are some real-world consequences?
- Unstable or deformed flanges.
- Inability to form the part as designed.
- Fit and assembly issues.
Guidelines and Numbers
A minimum of 4x the material thickness for the flange length.
What are the best practices?
- Ensure the flange length is at least 4x the material thickness.
- Check the press brake tooling to confirm the flange can be securely held and formed.
- Prevent deformation by increasing the flange length for thicker materials.
Omitting Bend Relief Cuts
What is the mistake, and why does it happen?
Failure to add relief notches at the intersection of bends and edges can induce tearing, bulging, or incomplete bends.
It’s a mistake to overlook the need for the material to stretch during bending, or to try to simplify the design.
What are some real-world consequences?
- Tearing or warping at bends.
- Deficient cosmetic appearance.
- Increased scrap in rework.
Guidelines and Numbers
- Bend Relief Width: Use a minimum of ≥ 50% of material thickness.
- Bend Relief Depth: A minimum bend radius + thickness + 0.020 in.
What are the best practices?
- Especially for thick materials or if complex bends are required, add reliefs at all the critical intersections.
- Allow the material to stretch without tearing by following the width and depth guides.
- For closed box bends and flange intersections, use reliefs.
Errors in Hems, Curls, and Other Forming Features
What is the mistake, and why does it happen?
Improper dimensions, ignoring grain direction, or placing features too close to bends or edges can be a mistake when designing hems, curls, gussets, dimples, or louvers.
These mistakes can happen when there is a lack of familiarity with forming limitations or not considering the material’s behavior.
What are some real-world consequences?
- Cracking or incomplete forming.
- Weak joints or poor fit.
- Warping or distortion.
Guidelines and Numbers
| Feature | Minimum/Recommended Value |
|---|---|
|
Hem Inside Diameter |
≥ Material Thickenss |
|
Hem Return Length |
6 x Material Thickness |
|
Curl Radius |
≥ Material Thickness |
|
Dimple/Louver Distance |
4 X Material Thickness From Bends/Edges |
What are the best practices?
- For manufacturability, use standard hem and curl dimensions.
- At least 4T distance to reinforce features away from bends and edges.
- To balance forming stresses, maintain symmetry.
- Design bends parallel to the grain’s direction where possible.
The wrong hardware and fasteners
What is the mistake, and why does it happen?
For example, placing PEM nuts, standoffs, or studs too close to the bends. Failing to provide tool clearance or using incompatible hardware and material combinations.
The mistake happens when installation requirements are overlooked or when the hardware manufacturer’s guidelines are not consulted.
What are some real-world consequences?
- Deformed holes or failed hardware installation.
- Weak joint or assembly failures.
- Costly rework or design.
Guidelines and Numbers
- Hardware Hole to Bend: 4x material thickness.
- Hardware Specifications: Call out the type, size, and installation methods.
- Hardware Compatibility: Sheet metal materials must be softer than the hardware for proper clinching.
What are the best practices?
- In both the design and assembly documentation, check the hardware clearance and accessibility.
- Specify the hardware type, size, and installation method.
- For compatibility and installation requirements, consult the manufacturer’s guidelines.
- If the hardware must be near the bends, add reliefs or cutouts.
Poor Surface Finish Selection and DFM oversights
What is the mistake, and why does it happen?
Specifying finishes that are incompatible with the base material or the application. Ignoring the thickness added by specific coatings. Over-specifying features that increase the cost and lead time can be mistakes.
It happens when there is a lack of awareness of the finishing processes, or if finishes are copied from other projects without considering material or function.
What are some real-world consequences?
- Poor corrosion resistance or cosmetic defects.
- Parts that don’t fit due to the coating thickness.
- Increased cost and production delays.
Guidelines and Numbers
| Material | Compatible Finishes | Notes |
|---|---|---|
|
Aluminum |
Anodizing, Chromate, and Powder Coat |
Anodizing is not for steel. |
|
Steel |
Powder Coat, Plating, and Painting |
Anodizing not suitable. |
|
Stainless |
Passivation, Polishing, and Plating |
Usually left natural. |
What are the best practices?
- Match the finish to the material and application. For example, don’t specify anodizing for steel.
- Especially for mating parts, adjust the tolerances for coating thickness.
- Avoid unnecessary features, like blind holes or tight tolerances that increase costs.
- Engage early in DFM reviews to catch and correct issues before production.
FAQs
What is sheet metal design?
Sheet metal design involves the creation of parts and components using flat sheets of metal that are then formed, cut, and assembled into the final product. This process allows for the efficient production of a wide range of products, from simple brackets to complex enclosures and housings. Key considerations in sheet metal design include material selection, thickness, bend radii, and fabrication methods.
What is sheet metal design hardware?
Sheet metal design hardware refers to the tools, equipment, and materials used in the design and fabrication of sheet metal components. This includes items such as metal forming dies, bending jigs, cutting tools, and fastening hardware. These elements are essential for creating precise and durable sheet metal parts for various applications.
How to design sheet metal in Solidworks?
To design sheet metal parts in Solidworks, follow these steps:
1. Start a new part file and select the “Sheet Metal” option.
2. Define the base flange by specifying the thickness, bend radius, and other parameters.
3. Use the “Edge Flange” and “Bend” features to create additional flanges and bends.
4. Utilize the “Cut” and “Hole” tools to add features like cutouts and holes.
5. Use the “Flatten” feature to view the unfolded sheet metal layout.
6. Apply appropriate materials and finishes to the part.
7. Generate detailed drawings and documentation for manufacturing.
