Plastic and Sheet Metal Bending and Forming Guidelines

We’ve covered everything you need to know about plastic and sheet metal bending and fabrication for your laser-cut and CNC routed parts from SendCutSend. You should also check out our Designing for Bending page.
Play Video

Table of Contents

Setup and Cost

Bending your metal and plastic parts adds a $19.00 minimum to your cart total.

Save up to 70% or more with quantity discounts! We calculate quantity discounts based on several factors including material, operation type, number of operations on each part and number of duplicate parts. Our app will automatically provide quantity discounts based on your order.

Check out our processing page for information about typical lead times for parts with bending and other services. We provide free 3-5 day shipping for standard orders (higher quantities may require additional time). Most bent parts will ship ground as they will exceed 2″ in height when packed.

Materials Available for Bending

Material Limits

  • 0.030” – 0.250” thickness
  • Minimum flat part size
  • Maximum flat part size
  • No 6061/7075 Aluminum
  • No Grade 5 Titanium
  • No AR400/AR500
  • No 1075 Spring Steel

Service and Material Limitations

Before you start dreaming up your next project, you’ll need to know some of the metal and plastic bending limitations.

General

  • Maximum flat part size 44″ x 30″
  • Maximum bend length 16″ – 44″ depending on material thickness
  • Maximum thickness of .250”, depending on flange length

  

Metal

  • Maximum bend angle will be limited to 90° for specific materials
  • Metal parts will have a +/- 1-2° angle tolerance depending on bend length

 

Polycarbonate

  • Polycarbonate parts will have a +/- 5-degree bend angle tolerance on bends up to 24″ long
  • Polycarbonate parts will have a +/- 7-degree bend angle tolerance on bends longer than 24″
  • Polycarbonate parts are limited to up to 3 bends or flanges per part. More than 3 bends will require a custom quote. 
  • Polycarbonate bends can be no greater than 90° and no less 45°

 

While we’re happy to bend your parts to your hearts’ desire, there are some bends we don’t offer:

  • No acute angles greater than 130°
  • No obtuse angles less than 5°
  • No curl, bump, or roll forming
  • No coining
  • No hemming
  • For polycarbonate parts,
    no joggle bends

Our Process: Air Bending

At SendCutSend we form sheet metal and plastic with air bending. While a flange is being formed, there are just three points of contact between the material and the tooling: the punch and two sides of the die. An air gap is present in the die’s trough under the flange’s apex, which gives the process its name.

Effect on Bend Radii

With air bending, the effective radius is determined by the tooling combination (die + punch) and a material’s thickness and strength. Depending on your material choice, the effective radius (the internal radius after bending) may be smaller for a thicker gauge, or vice versa. Our effective bend radii are listed on each material page under Material Details.

Polycarbonate Limitations

To bend polycarbonate, flanges must be overbent to achieve the desired angle due to the spring back of the material. This means that some designs that can be formed in sheet metal may not be feasible in plastic.

In the example shown here, the material is bent 120-130 degrees to achieve a 90-degree angle.

Die Line Considerations

Die lines are the full extent of the width of the tooling, or die, that we use to form parts. When a part is bent, witness marks are left where the die makes contact with the part. These points of contact are what we refer to as die lines.

These points of contact (witness marks) are what we refer to as die lines

The problem: feature distortion

While the effective bend radius for our materials ranges from .024″ – .250″, the dies we use will span at least .472″ -1.575″ across the bend line. We cannot offer cosmetic protection along the die lines, so holes, edges, and other cutouts are subject to distortion in the bending process. 

For example, a part cut from 0.104” mild steel will be bent with a 0.630” die. This means that any cut feature 0.315” or less away from the bend line (center of the bend) will be distorted in the forming process.

When ordering your part from us, we will show you the feature distortion caution area when you configure your bend angles. The hole in the yellow portion of this screenshot will be distorted.

You can measure the die width on your flat pattern before uploading your file. Reference the die width for your material from our material library. The center of the die width will fall on the bend line as shown in this example. 

.104″ Mild Steel
Die width: .630″

Solution

If features fall within the die line of our tooling, you should remove them or adjust their location. Check out each material page to see what die we will use for your material of choice, and make sure your cut features are at least half the die’s width away from the bend line.

Ensure all holes and cutouts on your design fall outside of the die width area. In the example below the holes on one side of the bend are in the distortion area, while the others are not.

Check out our Bending Deformation Guidelines for more information.

File Setup

Here are the basics you’ll need to know before you send us your first file for bending. If you have any questions, feel free to contact support.

Files Accepted by Our Instant Quote System:

Make sure the part design you upload for bending is either a 2D vector file (.dxf, .dwg, .ai, or .eps format) or a 3D .step or .stp format file. You will be able to view your bends in a 3D model during the checkout process to make sure the angles and flange orientations are correct.

SOFTWAREFORMATBEND LINE
Fusion360.dxf, .step, .stpSolid line (default)
Fusion360.aiSolid, separate color from cut lines
SolidWorks.dxf, .step, .stpDashed line
(not hidden)
AutoCAD.dxf, .step, .stpDashed line
(not hidden)
CorelDraw.epsSolid, separate color from cut lines
Inkscape.epsSolid, separate color from cut lines

Please upload either a 2D .dxf, .dwg, .ai, or .eps format vector file or a 3D .step or .stp format file with your part design. 

If you design your parts in non-CAD software (Adobe Illustrator), please send us the original (native) .ai file. We’ll take care of the conversion on our end. While we accept .ai and .eps files, it’s critical that your bend lines are parallel when uploaded from these softwares or the file will delay our process.

For the fastest turnaround on your order, we recommend designing your parts in CAD software.

To learn more about design guidelines for laser cut sheet metal, see our Laser Cutting Guidelines.

For CNC routed polycarbonate design guidelines, please see our CNC Machining Guidelines.

Working in Solidworks? Download our custom bend tables to specify exact bend allowances, bend deductions, and K-factors so your file is tailored to our manufacturing processes.

Flange and Base

Before we begin, some basic terms you’ll need to know are base and flange. The flange is the edge you will be bending.

Minimum and Maximum Flange Length

The minimum flange length will change depending on what material and thickness you use. Please reference your chosen material in our materials directory to see the correct dimensions under Material Details.

The example here shows the bending information for .040″ 5052 Aluminum. 

The maximum flange length for 4-sided box bends is 3.50″ if no hardware will be installed for all materials. With hardware, the maximum flange length is 3.00″. We have more information available here.

Maximum Flat Size

Maximum flat part size is 44″ x 30″. Flat size is the total of your base and flanges.

Bend Lines in 2D Files

If you upload a 2D vector file, we will use the flat .dxf (or .ai file if you use Adobe Illustrator) for cutting and bending, so please indicate your bend locations in your drawing using a line. Bend lines should mark the center of each bend. During the ordering process, you can specify bend angles for each line. You will receive an error message in the app if your bend line is missing or insufficient, 

Bend Deduction

Bend Deduction is used to counteract material stretch caused by forming. This is unique to each material type, thickness, and bend angle. We’ve created a calculator to help you make your measurements spot on.

Advanced-user note: All calculations should be for air bending, not coining.

Once you have your new measurements from the bend calculator, you’ll want to adjust your file accordingly. You will be reducing the length of your base and flange to accommodate the length of the bend itself, aka the bend deduction. See the illustration below for an example. The green line indicates where the bends will occur.

Measuring Formed Flange Lengths

Formed flange lengths should always be measured from the apex of the bend.

Acute and Obtuse Bends

The bend angle is measured on the outside of the bend. In the illustration below, you will see that the acute bend is being called out as 130°. Material stock thicknesses have minimum and maximum angle limits. You can confirm limits for each thickness on the material pages.

Note: the bend radius for your part can be found on the material page or the bending calculator. We do not offer a custom bend radius.

C-Channel or U-Channel Bends

Sheet Metal Parts

For these bends in sheet metal, the base must be at least 2 times wider than the flange length. For example, a 1” flange on two sides requires a minimum 2” base (base is the remaining material, or the “bottom of the U”). The base can be greater than 2:1. For example, a 5” base with 1” flanges is fine (that would be a 5:1 ratio).

Polycarbonate Parts

For these bends in polycarbonate, the base must be at least 3 times wider than the flange length (3:1 ratio).

Window or Joggle Bends

Sheet Metal Parts

Window bends and joggle bends are allowed up to 90° for sheet metal parts. More acute angles require review by our team. You can find the minimum and maximum joggle flange values on the charts for your chosen material.

Polycarbonate Parts

Joggle bends are not available for polycarbonate parts, however we can provide window bends up to 90°.

Parallel bends in opposite directions can be bent in polycarbonate as long as the flanges are at least 3″ apart if measuring from the center or apex of each bend, and one of the flanges is no longer than 5″.

Odd Flange Shape

While we do allow for irregular shapes for your flange, we will need a flat piece to bend. To do this, add tabs to make a flat surface parallel to the bend. Please see the example below for proper breakoff tab usage.

Correct Tab Setup

Incorrect Tab Setup

Breakoff Tab Length

  • We’ll need your breakoff tab to be a sufficient length relative to your part’s overall flat length. Please note, we may request a longer tab if needed for a successful bend, depending on your design’s geometry.
    • 0-5 inch part: 0.500″ minimum breakoff tab
    • 5-10 inch part: 1.000″ minimum breakoff tab
    • 10+ inches: 1.500″ minimum breakoff tab

Connecting Bridges

  • Please create a minimum of 2 connecting bridges from your part to the breakoff tab
  • Longer flanges will benefit from more bridges. We recommend the following:
    • 0-10 inch flange: minimum of 2 connecting bridges
    • For every additional 10 inches, add at least one more bridge
  • Ensure the connecting bridges are at least 0.040” wide or the minimum bridge width for the material; whichever is larger. If bridges are too thin, they may break during the bend operation.
  • When determining bridge width, keep in mind that you’ll need to remove the breakoff tabs when your parts get to you.
    • For materials 0.080” or thicker, we recommend that bridges are no wider than 50% of the material thickness.

Keep Outside of Die Lines

  • The breakoff tabs’ connecting bridges must not fall within the die lines. Tabs are vulnerable to breakage if the connecting bridges are within the die area.

Add To Exterior of Part

  • We need break-off tabs added to the exterior of parts since we are unable to use tabs placed on the interior of a part.

Bend Relief Notches

To reduce bulging in the corners of your bent parts and prevent tearing, you can incorporate bend relief notches into your design. Bend relief notches are just narrow notches or circles put into the corners of your design. These notches should be at least 50% of the material’s thickness in width and the depth should equal to Bend radius + Material thickness +.020”.

These notches allow for less stress on the inner radii of the flanges, and will help keep the corners of the bends from interfering with the base material. Check out our guide to designing bend reliefs and Bending Deformation Guidelines for more information.

Polycarbonate Considerations

Polycarbonate parts require the minimum bend relief necessary; otherwise, the material will crack when bent. Find the bend relief depth required for each polycarbonate sheet thickness here.

Since polycarbonate parts are overbent to achieve the desired angle, adjacent flanges bent in the same direction will require sufficient clearance to avoid collision.

Ensure you have adequate clearance to avoid collision

Another thing to note is that we require rectangular bend reliefs for Polycarbonate. Any transition in a corner will add stress and result in tearing.

Rectangular reliefs are recommended for Polycarbonate parts

What to Expect

General

  • Simple, single bend parts will have a +/- 0.015” tolerance, bend to edge
  • Multi bend parts will have a +/- 0.030” tolerance, bend to edge; each bend adds at least .015” tolerance
  • Witness marks from the bending process will be visible; these can become deeper and more noticeable depending on the material
  • We do not offer special protection for cosmetic parts at this time
  • Some bulging at the ends of the bend will be expected

Sheet metal

  • Sheet metal parts will have a +/- 1-degree bend angle tolerance on bends up to 24″ long
  • Sheet metal parts will have a +/- 2-degree bend angle tolerance on bends longer than 24″

Polycarbonate

  • Polycarbonate parts will have a +/- 5-degree bend angle tolerance on bends up to 24″ long
  • Polycarbonate parts will have a +/- 7-degree bend angle tolerance on bends longer than 24″
  • Polycarbonate parts may have minor surface edge cracks depending on the material thickness and bend angle
  • Polycarbonate parts will have noticeable cracking in stressed areas if adequate relief is not provided for each bend
  • Polycarbonate parts are limited to up to 3 bends or flanges per part. More than 3 bends will require a custom quote.
  • Polycarbonate bends can be no greater than 90° and no less than 45°
Witness marks from bending process

Common Issues

Combined Lines

Bends on a common axis need to be joined, as in the example shown here. If they are not joined, each bend will be seen individually.

Intersecting Bends

We are unable to bend intersecting lines that do not have separate flanges. Please reference the bending design guidelines.

Insufficient or Missing Bend Relief

Certain designs require bend relief to avoid damage to the part. Without proper relief, a part cannot be bent accurately. This is a critical consideration for polycarbonate parts since the material is prone to cracking. Check out our guide to designing bend reliefs and Bending Deformation Guidelines for more information.

You’re Ready to Bend

Although metal and plastic forming is a deeply complex process, we here at SendCutSend aim to make part bending as easy as possible. Questions? Reach out to our support team.

Happy bending!

Pre-flight Checklist

Additional Resources

Play Video
Play Video
Play Video
Play Video
Play Video
Play Video

Start your first SendCutSend project today!

Upload your CAD design or use our parts builder and get instant pricing on your custom laser cut parts, all delivered to your door in a matter of days.
No CAD File? No Problem! Send your sketch or template to our Design Services team. Starting at $49.

We proudly use hardware by PEM

Flush stud, M8 x 1.25, .472" Zinc plus Clear Chromate

Aluminum: 5052, 6061, 7075 Steel: Mild

SKUFH-M8-12
Thread SizeM8 x 1.25
Hole size in sheet (+0.003/-.0.000).315″
Minimum sheet thickness0.094″
Maximum sheet thickness.347″
Fastener materialSteel
Minimum distance hole C/L to edge0.378″
Minimum distance between two of the same hardware.567″
Recommended panel materialSteel/Aluminum
Coating typeZinc
Length.472″
Aluminum material ranges (5052, 6061, 7075)0.100″-0.250″
Steel material ranges (CRS, HRPO, HR)0.104″-0.250″

Get an Instant Quote for Waterjet Cutting

We proudly use hardware by PEM

Flush Standoff, 4-40, .250" Zinc plus Clear Chromate

Aluminum: 5052, 6061, 7075 Steel: Mild, G30

SKUSO-440-8
Thread Size4-40 x .250″
Hole size in sheet (+0.003/-.0.000).168″
Minimum sheet thickness0.040″
Maximum sheet thickness.125″
Fastener materialSteel
Minimum distance hole C/L to edge0.230″
When determining the distance between two or more fasteners, you can calculate the distance by the formula, C/L to edge + 1/2 the diameter of the second mounting hole..345″
Recommended panel materialSteel/Aluminum
Coating typeZinc
Length.250″
Aluminum material ranges (5052, 6061, 7075)0.040″-0.125″
Steel material ranges (CRS, HRPO, HR)0.048″-0.119″

We proudly use hardware by PEM

Flush Standoff, 4-40, .250" Passivated

Stainless Steel: 304, 316

SKUSO4-440-8
Thread Size440
Hole size in sheet (+0.003/-.0.000).166″
Minimum sheet thickness0.04″
Maximum sheet thickness.125″
Fastener material400 Stainless Steel
Minimum distance hole C/L to edge0.230″
When determining the distance between two or more fasteners, you can calculate the distance by the formula, C/L to edge + 1/2 the diameter of the second mounting hole. Example shown with x2 of the same hardware..313″
Recommended panel materialStainless Steel
Coating typePassivated
Length.250″
304 Stainless Steel material ranges0.048″-0.125″
316 Stainless Steel material ranges0.060″-0.125″