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.
Before you start dreaming up your next project, you’ll need to know some of the limitations to metal and plastic bending.
While we’re happy to bend your parts to your hearts’ desire, there are some bends we don’t offer:
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.
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 individual material page under Material Details.
In order to bend polycarbonate, flanges must be overbent to achieve the desired angle due to the springback 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 in order to achieve a 90 degree angle.
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.
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 distorting in the bend 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 that is 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 prior to 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″
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.
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.
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.
| SOFTWARE | FORMAT | BEND LINE |
| Fusion360 | .dxf, .step, .stp | Solid line (default) |
| Adobe Illustrator | .ai | Solid, separate color from cut lines |
| SolidWorks | .dxf, .step, .stp | Dashed line (default) |
| AutoCAD | .dxf, .step, .stp | Dashed line |
| CorelDraw | .eps | Solid, separate color from cut lines |
| Inkscape | .eps | Solid, 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 software or the file will delay our process.
For the fastest turnaround on your order, we recommend designing your parts in a 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.
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.
In any material, the maximum flange length for 4-sided box bends is 3.50″ if no hardware will be installed. With hardware, the maximum flange length is 3.00″. We have more information available here.
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.
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°. 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.
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.
Breakoff Tab Length
Connecting Bridges
Keep Outside of Die Lines
Add To Exterior of Part
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.
Since polycarbonate parts are overbent to achieve the desired angle, adjacent flanges bent in the same direction will require sufficient clearance to avoid collision.
We recommend providing clearance that is 1:1 to the material thickness.
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.
We are unable to bend intersecting lines that do not have separate flanges. Please reference the bending design guidelines.
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.
Although metal and plastic forming is a deeply complex process, we here at SendCutSend aim to make part bending as easy as possible. Questions? Email us anytime: support@sendcutsend.com
Happy bending!
No CAD File? No Problem! Send your sketch or template to our Design Services team.
We proudly use hardware by PEM
| SKU | FH-M8-12 |
| Thread Size | M8 x 1.25 |
| Hole size in sheet (+0.003/-.0.000) | .315″ |
| Minimum sheet thickness | 0.94″ |
| Maximum sheet thickness | .347″ |
| Fastener material | Steel |
| Minimum distance hole C/L to edge | 0.378″ |
| 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. | .535″ |
| Recommended panel material | Steel/Aluminum |
| Coating type | Zinc |
| Length | .472″ |
| Aluminum material ranges (5052, 6061, 7075) | 0.100″-0.250″ |
| Steel material ranges (CRS, HRPO, HR) | 0.104″-0.250″ |
We proudly use hardware by PEM
| SKU | SO-440-8 |
| Thread Size | 4-40 x .250″ |
| Hole size in sheet (+0.003/-.0.000) | .168″ |
| Minimum sheet thickness | 0.040″ |
| Maximum sheet thickness | .125″ |
| Fastener material | Steel |
| Minimum distance hole C/L to edge | 0.230″ |
| 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. | .314″ |
| Recommended panel material | Steel/Aluminum |
| Coating type | Zinc |
| Length | .250″ |
| Aluminum material ranges (5052, 6061, 7075) | 0.040″-0.125″ |
| Steel material ranges (CRS, HRPO, HR) | 0.048″-0.119″ |
