Xometry Sheet Metal Design Guide

User Manual:

Open the PDF directly: View PDF .
Page Count: 12

Download
Open PDF In Browser	View PDF

Design Guide: Sheet
Metal Fabrication
VERSI ON 2 .1

SHEET M ET AL GU I D E V 2 . 1

Table of Contents
Overview.................................................................................................3
Tolerances..............................................................................................4
General Tolerances.....................................................................................4
Wall Thickness..............................................................................................5
Bends........................................................................................................5
Curls................................................................................................................6
Countersinks.................................................................................................6
Hems.....................................................................................................................7
Holes & Slots.................................................................................................8
Notches & Tabs............................................................................................9

Features...............................................................................................10
Corner Fillets..............................................................................................10
Relief Cuts...................................................................................................10

Finishes & Post-Processing...............................................................11
Resources at Xometry.......................................................................12

2

SHEET M ET AL GU I D E V 2 . 1

Overview
Sheet metal fabrication is the process of forming parts
from a metal sheet by punching, cutting, stamping, and/
or bending. 3D CAD files are converted into machine
code, which controls a machine to precisely cut and
form the sheets into the final part. Sheet metal parts
are also known for their durability, which makes them
great for end-use applications (e.g. chassis). Parts used
for low volume prototypes, and high volume production
runs are most cost-effective due to large initial setup and
material costs.
Because parts are formed from a single sheet of metal,
designs must maintain a uniform thickness. Be sure to
follow design requirements and tolerances in this guide
to ensure parts fall closer to design intent.

3

SHEET M ET AL GU I D E V 2 . 1

Tolerances
General Tolerances
If a drawing or specification sheet has not been provided
by the customer, Xometry will manufacture the product
from the model to the specifications listed below:
• Forming and bending: +/- 0.020”
• Bend to hole or feature: +/- 0.010”
• Linear dimensions excluding locations to bends: +/0.005”
• Diameters with inserts: +0.003/-0
• Angularity: +/- 2 degrees
• Surface roughness (blank material): Ra 125 uin max
• Surface roughness (timesave): Ra 100 uin max

4

SHEET MET A L GUI DE V2 .1 — T OL ER A N C ES

Wall Thickness
Parts must maintain a uniform wall thickness throughout
their

entirety.

Generally,

Xometry

is

capable

of

manufacturing sheet metal parts up to ¼” (6.35mm) in
thickness, but this tolerance mainly depends on the
geometry of the part.
When considering sheet metal thickness, a single sheet with
punches (holes) is a good rule of thumb. Some features,
such as countersinks are doable, but counterbores and
other machined features are difficult to produce as they
require post-machining.
Drawing indicating uniform wall thickness

Model indicating uniform wall thickness

Bends
Sheet metal brakes are used to bend material into a part’s
desired geometry. Bends in the same plane should be
designed in the same direction to avoid part reorientation,
which will save both money and time. Keeping a consistent
bend radius will also make parts more cost-effective. Small
bends to large, thick parts tend to become inaccurate, so
they should be avoided if possible.

Inside bend radius

D IM E N S I ON S
To prevent parts from fracturing or having distortions,
make sure to keep inside bend radius at least one
material’s thickness.

5

Consistent bend
orientations

Inconsistent bend
orientations

SHEET MET A L GUI DE V2 .1 — T OL ER A N C ES

Curls
D IM E N S I ON S
Outside radius must be at least twice the material’s thickness.

C LE A R A N CE S
Holes should be placed away from the curl at least a
distance of the radius of the curl plus the material’s

Example of a curl

thickness. Bends should be at least 6 times the material’s
thickness plus the radius of the curl.

Countersinks
D IM E N S I ON S
The maximum depth a countersink may have is 3.5 times
the material’s thickness.
Example of a countersink

C LE A R A N CE S
Countersinks must be at least 8 times the material
thickness from each other, 4 times the material’s thickness
from an edge, and 3 times the material’s thickness from a
bend.

Center-to-center distance

Center-to-bend distance

6

SHEET MET A L GUI DE V2 .1 — T OL ER A N C ES

Hems
Hems are folds to the edge of a part to create a rounded,
safe edge. Hems may be open, flat, or tear-dropped, and
tolerances depend on the hem’s radius, material thickness,

Open hem

Tear-dropped hem

and features near the hem.

N OT E :
Flat hems risk fracturing the material at the
bend, and should be avoided if possible.

D IM E N S I ON S
For open hems, minimum inside diameter is equal to the
material thickness (larger diameters tend to lose circular

Open hem inside diameter

shape), and the return length is at least 4 times the
material’s thickness. Tear-dropped hems must maintain
an inside diameter of at least one material’s thickness, an
opening of at least ¼ the material’s thickness, and return
length is also 4 times the material’s thickness.

Open hem return length

Tear-dropped hem opening distance

7

SHEET MET A L GUI DE V2 .1 — T OL ER A N C ES

Holes & Slots
D IM E N S I ON S
Keep hole and slot diameters at least as large as material
thickness. Higher strength materials require larger diameters.

C LE A R A N CE S
Holes and slots may become deformed when placed near

Hole-to-bend distance

Slot-to-bend distance

Hole-to-edge distance

Slot-to-edge distance

a bend. The minimum distance they should be placed
from a bend depends on the material thickness, the bend
radius, and their diameter. Be sure to place holes away
from bends at a distance of at least 2.5 times the material’s
thickness plus the bend radius. Slots should be placed 4
times the material’s thickness plus the bend radius away
from the bend.
Be sure to place holes and slots at least 2 times the material’s
thickness away from an edge to avoid a “bulging” effect.
Holes should be placed at least 6 times the material’s
thickness apart.

8

SHEET MET A L GUI DE V2 .1 — T OL ER A N C ES

Notches & Tabs
D IM E N S I ON S
The minimum thickness a notch must maintain is at
least 0.04” (1mm) or the material’s thickness, whichever
is greater; the length must be no larger than 5 times its
width. Tabs must be at least 0.126” (3.2mm) thick, or two

Notch thickness

Notch length

Notch-to-bend
distance

Notch-to-notch
distance

Tab thickness

Tab-to-tab distance

times the material’s thickness, whichever is greater; the
length must also be no larger than 5 times its width.

C LE A R A N CE S
Notches must be at least ⅛” (3.175mm) away from each
other. For bends, notches must be at least 3 times the
material’s thickness plus the bend radius. Tabs must have
a minimum distance from each other of 0.04” (1mm) or the
material’s thickness, whichever is greater.

9

SHEET M ET AL GU I D E V 2 . 1

Features
Corner Fillets
Sheet metal parts may have sharp corners, but designing
a fillet of ½ the material’s thickness will make parts more
cost-effective.

Corner fillets

Relief Cuts
Relief cuts help parts fall closer to design intent to avoid
“overhangs” and tearing at bends. Overhangs become
more prominent for thicker parts with a smaller bend
radius, and may even be as large as ½ the material’s
thickness. Tearing may occur when bends are made close
to an edge.

D IM E N S I ON S
Relief cuts for bends must be at least one material’s
thickness in width, and must be longer than the bend radius.

Bend relief to prevent tearing

Bend relief to prevent “bulging”

10

SHEET M ET AL GU I D E V 2 . 1

Finishes & Post-Processing
Xometry offers sheet metal parts in a wide array of
materials including:
• Aluminum
• Stainless steel
• Bronze/Brass
• Copper
• Steel
To further customize parts, Xometry offers post-processing
options to add to sheet metal parts such as:
• Bead Blasting
• Plating
• Welding
• Inserts
• Other custom finishes upon request

11

SHEET M ET AL GU I D E V 2 . 1

Resources at Xometry
Online Instant Quoting

Live Engineering Support

Web: Upload your CAD file at get.xometry.com/quote

Hours: M-F 8:00 AM - 9:00 PM EST

CAD:

Email: support@xometry.com

Download

the

free

Xometry

Add-In

for

SOLIDWORKS: xometry.com/solidworks

Phone: (240) 252-1138

Accepted File Types: .stl, .step, .stp, .x_t, .x_b,

Online: xometry.com/support offers live chat, FAQs,

.sldpart, .ipt, .prt, .sat, .catpart (max file size: 300MB)

and other helpful articles.

Capabilities: CNC Machining, Sheet Metal Fabrication,
3D Printing, Urethane Casting, Injection Molding

ITAR Registered
All uploads are secure and confidential. Contact us for assistance with large orders and existing
Xometry quotes.
Need to use a PO? We offer same day credit application processing. Contact us for details.

12



---

Source Exif Data:

File Type                       : PDF
File Type Extension             : pdf
MIME Type                       : application/pdf
PDF Version                     : 1.7
Linearized                      : Yes
Language                        : en-US
XMP Toolkit                     : Adobe XMP Core 5.6-c143 79.161210, 2017/08/11-10:28:36
Create Date                     : 2018:01:18 10:40:59-05:00
Metadata Date                   : 2018:01:18 10:41:14-05:00
Modify Date                     : 2018:01:18 10:41:14-05:00
Creator Tool                    : Adobe InDesign CC 13.0 (Macintosh)
Instance ID                     : uuid:c739739e-efff-d54b-a361-32a635797279
Original Document ID            : xmp.did:ace6199e-779e-44d3-a047-ce44fa168d9f
Document ID                     : xmp.id:e9f086b9-5d97-4821-9c09-b7311a58761b
Rendition Class                 : proof:pdf
Derived From Instance ID        : xmp.iid:a79f720f-3c07-40c6-a091-145e3217e97d
Derived From Document ID        : xmp.did:dc25a8be-8f50-436b-baf5-3130f172b1a8
Derived From Original Document ID: xmp.did:ace6199e-779e-44d3-a047-ce44fa168d9f
Derived From Rendition Class    : default
History Action                  : converted
History Parameters              : from application/x-indesign to application/pdf
History Software Agent          : Adobe InDesign CC 13.0 (Macintosh)
History Changed                 : /
History When                    : 2018:01:18 10:40:59-05:00
Format                          : application/pdf
Producer                        : Adobe PDF Library 15.0
Trapped                         : False
Page Count                      : 12
Creator                         : Adobe InDesign CC 13.0 (Macintosh)

EXIF Metadata provided by EXIF.tools