To complete this section and all following sections, you will require a copy of the SolidWorks software program, along with basic working knowledge. This includes how to carry out operations such as starting new parts, creating and editing sketches and features, and using common tools. For readers who are completely new to SolidWorks, it is advisable to gain a firm foundation of solid modeling first, before undertaking the Sheet Metal module covered in this book.

During the course of the book, if a certain tutorial or tool is causing problems, then try double-checking all of the previous steps, or even try closing the part and starting again from the beginning.

Error messages in SolidWorks can be quite descriptive and often tell the user exactly what the issue is. So, if presented with an error, then try to avoid the temptation to click OK without reading it properly, and attempt to carry out the action suggested in the message.

If the problems persist, then feel free to contact me online via Twitter at www.twitter.com/johnoellison.

SolidWorks versions

The examples and demonstrations in this book were made using SolidWorks 2021. Other versions of SolidWorks may have very minor differences in things such as the interface and how certain options are labeled, but in general, the workflow should be very similar. If you do get stuck on any of these differences, then please contact me using the details previously provided.

Units of measurement

Throughout this book, millimeters (mm) are used as the unit of measurement, but this can be adjusted according to the reader's preference by setting the model's units to inches ("), for example, and then typing the millimeter numerical value followed by mm into the Smart Dimension tool when adding dimensions. This will automatically convert the millimeter values into inches (or your selected unit type).

Terminology

Throughout this book, "sheet metal" (lowercase) refers to the general industry and manufacturing methods used in the real world, whereas "Sheet Metal" (capitalized) refers specifically to the SolidWorks Sheet Metal module.

The term "part" refers to a real-life component or item, whereas part (italicized) refers specifically to a SolidWorks part document.

Sheet metal parts are those that are—as the name suggests—created from flat sheets of metal. Numerous different manufacturing techniques such as bending, cutting, and forming allow these simple flat sheets to be transformed into complex 3D parts. The popularity of sheet metal has exploded in modern times because it allows designers and engineers to take a widely available material type—the flat sheets—and use relatively low-cost tools and processes to create complex products, at an industrial scale.

The chances are that a quick look around your home, garage, or workplace will reveal dozens of items that were created using sheet metal techniques. These can range from very simple items such as right-angle brackets to more complex products such as furniture, all the way up to detailed designs such as computer or electronics enclosures. Sheet metal is also used to create very complex items such as aircraft parts or car bodywork, although the most advanced formed parts are beyond the scope of SolidWorks Sheet Metal.

Figure 1.1: Examples of sheet metal parts

The beauty of the SolidWorks Sheet Metal module is that it allows users to create these 3D shapes, then flatten them down to sheets, and export them as two-dimensional (2D) designs that can be used for manufacturing.

Another great aspect of SolidWorks Sheet Metal is that, despite the name, it doesn't have to be used for purely metal parts. Sheet Metal can be used to create any kind of flattened 3D part, regardless of the real-life material. Try to think beyond the "metal" title, and a wide range of other uses can be unlocked. For example, Sheet Metal can be used to create cardboard packaging. This can be modeled in 3D before being virtually unfolded to be printed, cut out with a die-cutter, and then turned into 3D boxes. Sheet Metal can also even be used to create items as diverse as paper origami artwork.

Figure 1.2: Sheet Metal isn't just for metal but any material, such as this cardboard packaging

Sheet Metal is a diverse set of manufacturing methods that will take your modeling and design to the next level. In summary:

• Sheet metal uses flat sheets to create 2D or 3D parts.
• Techniques include cutting, bending, and forming.
• SolidWorks Sheet Metal parts don't have to be metal!

In the next section, we'll look at how we can actually start making Sheet Metal parts in SolidWorks by creating a Base Flange that will be the foundation feature of these parts.

SolidWorks Sheet Metal parts can be started in two main ways—either by creating a Base Flange or by converting existing 3D parts into Sheet Metal parts. This section will cover the use of Base Flanges, which are the simplest but also the most flexible way to start new Sheet Metal parts.

Setting up the workspace

Before learning more about Base Flanges, let's first ensure that the workspace is set up correctly for Sheet Metal modeling. The Sheet Metal tools can be found via the Insert menu on the top menu bar (Figure 1.3) but it is faster and more convenient to use the Sheet Metal tab or toolbar:

Figure 1.3: The Sheet Metal tools in the Insert menu

Setting up the Sheet Metal tab or toolbar

To add the Sheet Metal tab, proceed as follows:

1. From within a SolidWorks part document, right-click on any of the existing tabs, or in any empty space, on the Command Manager (labeled i in Figure 1.4).
2. Select the Tabs sub-option (labeled ii in Figure 1.4) and ensure that there is a check mark next to the Sheet Metal option (labeled iii in Figure 1.4).

Figure 1.4: Adding the Sheet Metal tab to the Command Manager

This will then add the Sheet Metal tab to the existing tabs of the Command Manager.

To add the Sheet Metal toolbar:

1. The Sheet Metal toolbar can be added in a similar way to the tab. First, right-click on any of the existing tabs, or in an empty space, on the Command Manager (labeled i in Figure 1.4).
2. Select the Toolbars sub-option and ensure that there is a check mark next to the Sheet Metal option.

   Should You Use the Sheet Metal Toolbar or the Sheet Metal Tab?

   By default, the Sheet Metal tab and toolbar both contain the same set of tools. Either can be used throughout the book and this is a matter of user preference.

   The Sheet Metal tab contains larger, clearer icons, but the toolbar can be moved into the Graphics Area for easier access to tools.

Making a Base Flange

A Base Flange is the first feature of a Sheet Metal part and is the simplest way to create new Sheet Metal parts, while also offering the most flexibility. This is because once a Base Flange has been created, additional features such as bends and flanges can be added to build up a 3D part in a similar way to standard solid modeling. By contrast, converting existing parts to Sheet Metal (as covered later in the book) can limit the type of part that can be created and reduce editing options at later stages.

To actually create a Base Flange, a profile first needs to be sketched. Various profile types can be used, but this section will cover the simplest: a Single Closed profile.

To create a Base Flange:

1. Start a new SolidWorks part.
2. Start a sketch on the appropriate Plane, such as the Top Plane (labeled i in Figure 1.5).
3. Sketch the Base Flange profile. Different profile types will be covered later in the chapter, but for now, simply create a closed profile, such as a Center Rectangle (labeled ii in Figure 1.5).
4. Fully Define the profile by using the Smart Dimension tool and linking it to the Origin (labeled iii in Figure 1.5). Make the rectangle 200mm high and 300mm wide.

   Fully Defining Sketches

   During SolidWorks modeling, it is important to Fully Define sketches to ensure that the Sketch Entities are fixed and will not behave in unexpected ways, such as moving position. Fully Defined Sketch Entities will turn black, and when a sketch is Fully Defined, this will be indicated in the lower right of the screen (labeled iv in Figure 1.5).

Figure 1.5: Sketching the Base Flange profile

5. Exit the sketch (labeled v in Figure 1.5).
6. Select the Sheet Metal tab or toolbar and select the Base Flange/Tab option—this should be the first icon (labeled i in Figure 1.6).
7. You will be prompted to select a sketch. Select the previous sketch that was just drawn and a yellow preview of the Base Flange should appear (see Figure 1.6).

   Note

   It is also possible to skip Step 5 and select the Base Flange/Tab option directly from within the sketch. In this case, the sketch that is being edited will automatically be used.

8. Enter the following settings (these will be covered in more detail later in the chapter):
   • Thickness: 1mm
   • Bend Allowance: K-Factor, 0.5
   • Auto Relief: Rectangular
   • Ratio:0.5 (labeled iii in Figure 1.6)

Press OK (labeled iv in Figure 1.6) and the Base Flange feature is created.

Figure 1.6: Creating a Base Flange feature

The Base Flange feature is now created, and Base-Flange1 (note: your number may differ) appears in the FeatureManager Design Tree at the left of the screen (labeled i in Figure 1.7). This feature can be edited and adjusted in the usual way by left-clicking on the feature and selecting Edit Feature.

Creating a Base Flange feature turns the entire part into a Sheet Metal part and so automatically adds some extra items to the FeatureManager Design Tree. These items indicate that a part is a Sheet Metal model, and they are made up of the following:

• Sheet-Metal folder: This contains all of the global properties of your Sheet Metal part, such as the Thickness and the Bend Radius properties (labeled ii in Figure 1.7).
• Flat-Pattern folder: This folder contains a flattened version of the part (labeled iii in Figure 1.7). By default, this folder will be suppressed, so it will appear grayed out at this stage, but this will be covered in more detail later in the chapter.
• Cut list folder: This folder contains all of the separate sheets that make up the part. It can be thought of in a similar way to the Solid Bodies folder that is used in normal solid modeling

The number in brackets after the folder name indicates how many sheets make up the part. For example, a part with two separate body and lid sheets would show (2) after the Cut list folder (labeled iv in Figure 1.7).

Figure 1.7: Sheet Metal part details

Base Flanges are usually the best way of starting your Sheet Metal parts and are often the first feature created in a Sheet Metal part. They can be made by sketching a closed profile, then selecting the Base Flange/Tab option from the Sheet Metal tools.

Adding a Base Flange feature will turn the part into a Sheet Metal part and will automatically add the Flat-Pattern, Cut list, and Sheet-Metal folders, which we will explore more in the following section.

Saving Parts

At this stage, your current part can be saved as we will continue using this document throughout the book.

When working in SolidWorks, try to get into the habit of regularly saving your work, as a safeguard against crashes and other problems.

Sheet Metal properties are global settings that apply to the entire part. This section shows how to adjust these properties and what they actually mean. The section contains some background theory that is fairly dry but is an important foundation for understanding Sheet Metal. Some of this underlying theory will become much clearer once we actually start to use and demonstrate the tools later in the book, so don't worry too much if certain parts of it still appear a little confusing at this stage.

There are four Sheet Metal properties:

1. Sheet Thickness
2. Bend Radius
3. Bend Allowance
4. Auto Relief

Editing the Sheet Metal properties and adjusting the Sheet Thickness

As previously mentioned, Sheet Metal parts are usually made from sheets with a constant thickness. Therefore, the thickness of a part is an important aspect of Sheet Metal.

To edit the Sheet Metal properties of a part, simply left- or right-click on the Sheet-Metal folder in the FeatureManager Design Tree (labeled ii in Figure 1.7) and select Edit Feature.

To set the thickness, adjust the value under the Thickness field (labeled i in Figure 1.8) and press the green OK check mark. For example, try setting 2mm thickness and pressing OK. You should now see that the thickness of the Base Flange has changed from 1mm to 2mm.

Figure 1.8: Sheet Metal properties

This Thickness setting is global throughout the entire part, so any new features that are added, such as Edge Flanges, will also be made using this same thickness. Editing one single value in the Sheet-Metal folder provides a very simple way to adjust the entire part and all of the features that make it up.

Editing the Bend Radius

Along with the thickness, another very important property of Sheet Metal parts is the Bend Radius.

Whenever a flat sheet of metal is bent or folded to create 3D parts, the corners that are created by the bending process will never be completely square. Even with a very thin and flexible material, such as aluminium foil, a small bend radius is needed.

This is also true in SolidWorks Sheet Metal: a bend radius is always required (Figure 1.9), even if it is tiny.

Figure 1.9: A bend radius is always needed

In SolidWorks Sheet Metal the Bend Radius refers to the size of the inside of bends, and it can be set in the Sheet Metal properties.

Simply edit the Sheet Metal properties and adjust the value (labeled ii in Figure 1.8).

By default, the Bend Radius that is set in the Sheet Metal properties will apply to any features that are added to the part, although the Bend Radius can be overridden for specific bends, and this will be covered later in the book.

What size should we set the Bend Radius to?

Although setting the Bend Radius value itself is straightforward, how do we actually know what value to use for it? Bend Radius depends on a number of factors, such as the material type, the manufacturing method, and the thickness of the material. In general, as the sheet thickness increases, the bend radius value also increases. To visualize this, think about bending a very thin sheet of metal foil, compared to bending a thick plate—the thinner sheet will allow a much tighter bend to be created.

General figures for steel bending might be something like this:

There are a number of ways to determine the Bend Radius.

• Speak to your manufacturer. The most reliable method of determining the Bend Radius is usually to talk directly to the people making your parts. Tell them what you're planning to create, and the material type and thickness, and they should be able to recommend certain settings to use.
• Search online or in reference books. Try searching for a phrase such as 1mm thick steel bending radius. The results should give you a good idea of suitable values to start your design, which can then be fine-tuned at a later stage by adjusting the Sheet Metal properties.
• Use the SolidWorks Gauge Tables. Gauge numbers are a way of measuring the thickness of metal sheets based on weight. SolidWorks contains gauge tables that are a list of preset sizes that are built into SolidWorks Sheet Metal. They can be used to find common Bend Radius values.

To activate the Gauge Tables:

1. Put a check in the Use gauge table box at the top of the Sheet Metal properties (labeled iii in Figure 1.8). A table can then be selected from the drop-down list.

Note

SolidWorks Gauge Tables require Microsoft Excel to be installed on the computer and will not work without it.

2. Try selecting a table such as the SAMPLE TABLE – STEEL (Figure 1.10). The thickness of the Sheet Metal part can now be set using the gauge numbers from the dropdown list, rather than the specific thickness value.
3. Experiment with different sizes to see how the gauge number relates to actual thickness:

Figure 1.10: Using the Gauge Tables

Note

A higher gauge number corresponds to a thinner sheet. It can be seen in Figure 1.10 that 4 Gauge steel is 5.69mm thick, whereas 16 Gauge steel is only 1.51mm thick.

As the gauge number is changed, you'll notice that the Bend Radius value also automatically changes to correspond to the new sheet sizes. As expected, thicker sheets require a higher Bend Radius value.

Exercise Caution When Using Gauge Numbers!

Gauge numbers are specific to the material used, so confusion is easily caused. For example, a given gauge number of steel is not the same thickness as one in aluminum. 16 Gauge steel is 1.52mm thick, but 16 Gauge aluminum is only 1.29mm thick. For this reason, many international standards organizations recommend against the use of gauge numbers and instead suggest specifying the sheet thickness using dimensions.

The Gauge Tables can give a good indication of bend radii, but I recommend using them as a guide only, and instead directly setting and specifying sheet thicknesses.

The Bend Radius is a vital aspect of SolidWorks Sheet Metal and is needed for every bent part. It can be set in the Sheet Metal properties as a global value, but can also be overridden for certain bends if needed.

Get an idea of the Bend Radius needed by either speaking to your manufacturer, searching online, or using Gauge Tables. However, if using gauge numbers and tables, be careful to ensure your material choice is correct and clearly marked on any drawings. It is wise to use gauge tables as a guide only, and instead (or in addition to this) specify an exact sheet thickness.

Understanding the Bend Allowance

The next Sheet Metal property that affects your models is the Bend Allowance property (labeled iv in Figure 1.8). This allows us to accurately calculate the size of bent parts once they have been unfolded into a flat sheet.

To understand what exactly the Bend Allowance property is and why it is important, let's look at a simple part from the side. This consists of a Base Flange and one single Edge Flange, as illustrated in Figure 1.11.

Figure 1.11: Understanding the Bend Allowance property

We can see that the size of the Sheet Metal part will be the length of the Base Flange (A in Figure 1.11) plus the length of the Edge Flange (B in Figure 1.11), plus the size of the area of the bend itself (BA or Bend Allowance in Figure 1.11). Therefore, when the part is flattened, the total size of the sheet that we require will be A + B + BA.

However, depending on how and where the bend length (BA) is measured, we may end up with different values. For example, if the inside of the bend is measured, the length may be 5mm, but if the outside of the bend is measured then the length will be longer— 15mm in this case, as illustrated in Figure 1.12.

Figure 1.12: The size of the bend depends on where exactly is measured

The length of BA is determined by the Bend Allowance in the Sheet Metal properties, and there are a number of different options to set the Bend Allowance.

These Bend Allowance options are:

• Bend Table
• K-Factor
• Bend Allowance
• Bend Deduction
• Bend Calculation

Each option will give slightly different end results, but if you're unsure which option to use, then it's usually best to use the K-Factor bend allowance.

What Is the K-Factor Bend Allowance?

K-Factor is a way of working out the size needed for bends in sheet metal. Whenever a metal sheet is bent, there will always be a region of the bend, inside the bend, where the material is compressed, and another region, outside of the bend, where the material is stretched. At a certain point within a cross-section of the sheet, there will be a boundary where the compression and stretching exactly cancel each other out. Along this boundary, there will be no change of length in the material. The K-Factor is the name given to a line along this boundary, where no change in length occurs between flat and folded parts (Figure 1.13).

Figure 1.13: The K-Factor is an imaginary line through a cross-section of the material, where there is no change in size between the bent part and the flat part

The K-Factor is a ratio, so it will always be between 0 and 1. The inside of the bend is a K-Factor of 0 and the outside of the bend is a K-Factor of 1. Therefore, the middle of the bend is a K-Factor of 0.5, as illustrated in Figure 1.14.

Figure 1.14: The K-Factor is a ratio indicating a line through a cross-section of the bend

What Value of K-Factor Should I Use?

The K-Factor depends on a number of factors, such as material and bending type. If you're unsure about what to use, then a K-Factor of 0.5 is usually a good estimate for most parts and materials.

You can also try asking your manufacturer what value they recommend you should use.

The K-Factor is the easiest way to work out Bend Allowances and can easily be changed at a later stage if needed, by editing the Sheet Metal properties.

Other Bend Allowance options

As well as the K-Factor, there are also some other ways of calculating the Bend Allowance. If you are unfamiliar with these methods, then it is highly recommended that you use the K-Factor option, as detailed previously. The other Bend Allowance options are:

• Bend Allowance: This allows you to specifically define the length of the Bend Allowance. This can be useful if a manufacturer gives you a certain value to use. However, this option should be used with care as any value can be inputted. Therefore, if an incorrect value is used, this can result in completely wrong sizes on Flat Pattern parts.
• Bend Deduction: This option is somewhat similar to the Bend Allowance option but it measures the outside length of the folded part, then removes (or deducts) a certain value. Again, if you are unfamiliar with this method, use it cautiously, as using the wrong Bend Deduction value can give unusable results.
• Bend Table: This option allows a Bend Table to be created in Microsoft Excel. This table can specify Bend Allowance or Deduction values based on exact bend details, such as the radius and angle.
• Bend Calculation: Finally, the Bend Calculation option allows the use of equations to calculate the bending allowance based on factors such as the material's thickness, K-Factor, and the bend radius.

The Bend Allowance option is an important factor in ensuring that you are able to use the correct size of flat sheet to make your final, bent parts. A number of options are available, but if you're unfamiliar with Bend Allowance, then it is recommended that you simply use the K-Factor option. A K-Factor value of 0.5 gives a good estimation for most parts, and your manufacturer should be able to advise you in more detail, based on the material type and your exact part details.

Auto Relief options

The final Sheet Metal property is Auto Relief. This is a way of automatically adding relief cuts to bends if they are required. Figure 1.15 shows a simple Base Flange with an Edge Flange that only runs part of the way along the edge. In order to create this specific type of bend, Auto Relief cuts are needed; otherwise, the metal won't be able to bend correctly:

Figure 1.15: An example of an Auto Relief cut

Auto Relief cuts aren't needed on all bend types and will be automatically added when they are required. However, the exact type of relief cut is what is specified in the Auto Relief option.

The three types are:

• Rectangular: This gives a rectangular cut (see Figure 1.16). The size of the cut is determined by the ratio number and is related to the thickness of the sheet—for example, a ratio of 0.5 and a sheet thickness of 1mm will give a relief cut 0.5mm wide, which extends 0.5mm beyond the bend region. Note: the relief ratio has to be between 0.05 and 2.0.
• Obround: This gives a more rounded cut (see Figure 1.16) and also uses a ratio based on the thickness of the sheet in the same way as the Rectangular option.
• Tear: This option essentially tears the metal, without providing a visible cut area. This is the minimum that is needed to be able to flatten and bend the part.

All three options are depicted here:

Figure 1.16: Auto Relief examples; left to right: Rectangular, Obround, Tear

Auto Relief cuts are an important requirement for some bend types but they will be added automatically, so this option can usually be set to Rectangular or Obround with a ratio of 0.5 unless you have specific requirements.

A recap of Sheet Metal properties

Sheet Metal properties are an important way of defining your Sheet Metal part. They can be adjusted by editing the Sheet-Metal folder within the FeatureManager Design Tree. They generally apply to the whole part, although they can often be overridden for specific features.

The four options are:

• Thickness: This determines the thickness of the sheet used to create the Base Flange and subsequent features.
• Bend Radius: This sets the internal size of bends. A Bend Radius is always required for bent edges in SolidWorks Sheet Metal.
• Bend Allowance: This allows us to accurately calculate the correct size of flat sheet that can be used to create bent parts. There are a number of ways to calculate the Bend Allowance, but if you are unsure, then the best option is usually a K-Factor value of 0.5.
• Auto Relief: Some bends require relief cuts in order for them to be flattened or folded correctly. These will be added automatically if needed, but this option controls the size and type of cut.

Now that we have learned the basics of Sheet Metal properties and creating Base Flanges, we can go on to explore how 3D parts can be flattened, as well as more advanced types of Base Flanges.

In the previous section, we introduced Base Flanges, which are usually the first feature of your Sheet Metal part. As an example, we sketched a simple rectangle and then used this to make a rectangular Base Flange. This type of Base Flange is called a Single Closed profile because it only contains one single profile and that profile is closed (that is, it has no open areas or gaps in the outer perimeter). This can be seen in Figure 1.17.

Figure 1.17: A Single Closed profile contains one single profile, which is closed

However, two other options can be useful for creating different kinds of Base Flanges. These are the Multiple Contained Closed and the Single Open Contour profiles. It's not too important to remember the specific names, as long as you know how to use each type.

Multiple Contained Closed

For our previous Base Flange, we just used one single closed profile, but closed profiles can also contain other closed profiles within them. This type is known as Multiple Contained Closed and can be useful for adding holes and cutouts to your Base Flange. An example of this is shown in Figure 1.18.

Figure 1.18: Multiple Contained Closed Base Flanges can contain smaller closed profiles within one larger closed profile

Although using the Multiple Contained Closed option for creating Base Flanges can sometimes save time, I would personally recommend creating very simple Base Flanges and then adding extra cutouts and holes as separate features. This approach just makes it easier to adjust or remove extra details later on, if needed.

Single Open Contour

Instead of using closed profiles, it is also possible to create Base Flanges using open profiles known as Single Open Contours. These can range from a simple, single line, up to more complex collections of Sketch Entities.

To create a basic Single Closed Contour Base Flange:

1. Start a new part document and start a sketch on the appropriate Plane, such as the Front Plane.
2. Sketch the Base Flange. It can be easiest to think of the Single Open Contour option as a side view or cross-section view of the flange. For the first example, try a single horizontal line, 100mm long, using the Line tool (see Figure 1.19).
3. Remember to Fully Define your sketch by starting from the Origin and using the Smart Dimension tool to set the line's length.

Figure 1.19: Using a single-line sketch to create a Single Open Contour Base Flange

4. Select the Base Flange/Tab option from the Sheet Metal tab or toolbar.
5. The width of the Base Flange can be set using the Direction 1 (and Direction 2, if required) options in the Property Manager on the left of the screen. The Sheet Metal properties can also be set at this stage (see Figure 1.20).

Figure 1.20: Creating a Base Flange

6. Press OK to create a Base Flange. It can be seen that this creates a simple, rectangular Base Flange similar to the Single Closed Profile example from the first section.

In this way, the Single Open Contour Base Flange can be thought of as similar to the Thin Feature Extrude option from normal solid modeling.

Creating more Base Flange complex shapes

The real beauty of using the Single Open Contour option is that it allows you to easily create more complex, bent shapes in one feature.

1. Start a new part document and start a sketch on the appropriate Plane, such as the Front Plane.
2. Sketch a more complex shape using the Line tool. An example Z or jog shape can be seen in Figure 1.21.

Figure 1.21: A more complex Single Open Contour sketch

3. Select Base Flange/Tab from the Sheet Metal tools and set your desired options. Example settings could be:
   • Width: 10mm, Direction 1
   • Thickness: 2mm
   • Bend Radius: 1mm
4. Press OK to create a Base Flange (Figure 1.22). It can be seen that although the underlying sketch had sharp corners, the actual Base Flange feature has automatically been created with the bent corners using the Bend Radius that was specified in the Sheet Metal properties:

Figure 1.22: Single Open Contour Base Flange

Using Single Open Contours to create Base Flanges can be a good way to simplify the production of parts such as simple brackets.

Note that these types of sketches don't just need to use straight lines—they can also use arcs and splines if required.

Flattening parts

Now that we have created a part with bends in it, we can explore how 3D Sheet Metal parts can be flattened. Flattening is one of the features of the SolidWorks Sheet Metal module that really does add huge value to the design process because it allows parts to be accurately converted from finished parts into a state that can be easily created from sheets of flat stock material.

To flatten Sheet Metal parts:

1. From within a Sheet Metal part, select the Flatten option from the Sheet Metal tab or toolbar (labeled i in Figure 1.23).
2. The part will be unfolded into a flat sheet. Note the dotted outline, which indicates the bounding box of the flattened part, and the sketch lines, which show the location of Bend Lines (labeled ii in Figure 1.23).
3. If your Bend Lines aren't visible, try going to View | Hide/Show | Sketches.
4. Note also that the Flat-Pattern folder at the end of the FeatureManager Design Tree is now unsuppressed and so is no longer grayed out (labeled iii in Figure 1.23).

Using the Flatten option essentially unsuppresses (or switches on) the Flat-Pattern folder, which flattens the part. If you expand the Flat-Pattern folder, then the Flat Pattern feature will be seen, and this contains the bend details of the part.

5. To unflatten—or fold up—the part, simply click the Flatten button on the Sheet Metal tab or toolbar again or click the Flatten button that can be seen in the top right of the graphics area (labeled iv in Figure 1.23). Note that the part folds up and the Flat-Pattern folder is now suppressed (or switched off) again.

Figure 1.23: Flatten option

The Flatten option is a vital aspect of SolidWorks Sheet Metal that allows parts to be unfolded. As we progress through the book and learn about the Sheet Metal tools, we will see this option in use in a more practical setting.

A recap of Base Flange options and flattening parts

There are three types of Base Flange (See Fig. 1.24):

1. Single Closed Profile: This is one of the most basic types of Base Flange and uses one single profile that is fully closed, such as a simple rectangle or square. Although it is simple, this type of Base Flange is extremely useful and is likely to make up the majority of Base Flanges for Sheet Metal parts.
2. Multiple Contained Closed: Closed profiles can also contain smaller, closed profiles such as cutouts and holes. While these types of Base Flanges can be useful in certain situations, it is generally better practice to create simple Base Flanges using a Single Closed Profile and then add any extra holes, cuts, or details as separate features. This makes modification of these features at a later stage much easier.
3. Single Open Contour: Base Flanges can also be created using a collection of single Sketch Entities such as lines, arcs, and splines. This type of Base Flange can be useful when creating items such as brackets.

Figure 1.24: Types of Base Flange; left to right: Single Closed Profile, Multiple Contained Closed, Single Open Contour

Flattening is a vital aspect of SolidWorks Sheet Metal and parts with bends can be flattened by simply selecting the Flatten option from the Sheet Metal tools. This will unsuppress the Flat-Pattern folder and unfold any bends in the part.

So far in this chapter, we have learned how to start Sheet Metal parts and how to create the first feature of most of these parts—the Base Flange. We have also looked at how to edit the various Sheet Metal properties that are important to those parts. So, now that we have a reasonable idea of how to start virtual Sheet Metal parts, we will jump briefly into a real-world aspect of sheet metal and take a look at the various sheet metal materials available.

There are dozens of types of metal that could be used to create sheet metal parts and these all vary in use, physical properties, cost, and availability. The following pages will give you an idea of which might be best for your project.

This section is not an exhaustive list of materials; rather, it is just an overview of some of the most common ones that you are likely to encounter. Within these materials, there are also many specific grades (sub-types) of metal, each with slightly different properties. If in doubt, discuss your needs and budget with your sheet metal manufacturer and your material supplier to find the most suitable choice for your needs.

Steel and aluminum

The vast majority of sheet metal parts around us are made from either steel or aluminum, and of those, steel is probably the most common material.

Advantages and disadvantages of steel

Steel is an excellent all-round material, and if you're unsure which material to use, then steel is usually a solid choice. Steel is so popular and widely used for a number of reasons. It is very strong, easy to weld, and ductile, which means it is easy to bend and form compared to more exotic metals. Steel is also fairly inexpensive—it can be up to three times cheaper than aluminum for the same weight—and is widely available.

Material choice is always about compromise, so every material will have disadvantages. One of the main downsides of steel is that it is quite heavy—around two and a half times denser than aluminum, depending on the exact grades used. This means that if you have two pieces that are the exact same size and shape, then the steel part will be significantly heavier than the aluminum part.

Steel also has poor corrosion protection, meaning that it often goes rusty. You will have seen rusty steel items such as car bodywork. This rust is corrosion that is caused by a reaction between the metal and elements in the environment such as water and oxygen. The rust weakens and eventually destroys the metal. Steel can be treated to prevent or slow corrosion, but this will add to the material cost, and some other metals have much more natural resistance to corrosion.

Pros and cons of aluminum

Aluminum is the second-most common material used in sheet metal and is used in a wide range of items including bike frames, aircraft parts, and drinking cans.

One of the reasons why aluminum is so popular in the aerospace industry is that it is much lighter than steel. It also has excellent natural resistance to corrosion and so doesn't need extra surface treatments to stop it from going rusty. Another great property of aluminum is how malleable it is, meaning that it is very easy to bend. Consider how flexible aluminum foil is, or how easy it is to crush a drinks can.

Unfortunately, these positive properties also come with downsides, and aluminum is a lot more expensive than steel. However, because it is less dense, parts can be made lighter, which somewhat offsets this cost. Another factor is that although aluminum is lighter than steel, it is also weaker, meaning that parts that bear the same load will have to be made thicker in aluminum. However, due to the lower density of aluminum, these can actually be lighter than the equivalent steel parts. So overall, depending on exactly which grades of metal are used, aluminum generally has a better strength-to-weight ratio (SWR) than steel.

Other common metals

Steel and aluminum make up the vast majority of sheet metal parts but some other materials are reasonably common, such as the following:

• Copper: Copper is often used for parts such as electronics or heat-exchanging components because it has good electrical and thermal conductivity.

It is also easy to bend and form and has good corrosion resistance, and so is often used in plumbing, to make pipes and fixtures. Copper is more expensive than steel and aluminum, and some areas have issues with copper theft due to the higher price of the metal.

• Brass: This metal is an alloy (a mixture) of copper and zinc that looks similar to copper but has a brighter, shinier look. For this reason, it is often used for decorative items such as door knockers, fixtures, and trinkets.

It is extremely malleable and so is commonly used to make musical instruments in the brass section, such as trumpets. Brass has exceptional corrosion resistance and so is often seen in extreme environments, like door handles on ships. As with copper, it is quite an expensive metal and so is usually used sparingly.

• Stainless steel: Steel can be alloyed with other metals such as chromium to create different grades of stainless steel. This is steel that has a much greater resistance to corrosion than standard steel, while still retaining much of the strength and other benefits. For this reason, it is often used to make cutlery or surgical instruments.

Stainless steel sheet metal parts include things like large items of kitchen equipment—for example, sinks and countertops. However, this improved corrosion resistance makes stainless steel much more expensive than standard steel.

This overview is not intended to be a complete list of metals, and other niche materials might include tin, gold, and titanium. Each of these will have specific properties that suit different applications and budgets. As mentioned earlier, it is wise to discuss your specific needs with your sheet metal supplier and manufacturer to get the best fit for your project.

A summary of sheet metal material properties can be seen in the following table:

Sheet metal thicknesses and sheet sizes

Depending on where you live in the world, sheet metal is usually sold either by gauge number or the actual thickness of the sheet. As previously mentioned, gauge numbers are a way of measuring sheet metal thickness based on the weight of the material, and generally, a higher gauge number means a thinner sheet.

Gauge numbers are specific for each material, so 16 gauge steel will be a different thickness than 16 gauge aluminum. Therefore, it is highly recommended that sheet thickness is also specified in actual thickness, to avoid any confusion.

Metal sheets are also available in a wide range of sheet sizes, both metric and imperial. Some common sizes are shown in Figure 1.26 and include 48x120 " or 2x1 meters (m):

Figure 1.25: Common metal sheet sizes

When creating very big parts, or even large numbers of small parts, it is worth checking which sheet sizes are available to you and designing with this in mind. If making lots of small parts, it is even possible to use third-party "nesting" software to arrange the parts on the sheet in the most efficient way and avoid wasted material.

Material selection recap

Even when designing parts virtually in SolidWorks, it is important to consider how those parts will be created in the real world, and a vital aspect of this is the material choice. Most sheet metal parts are made from steel or aluminum, but other common metals include copper, brass, and stainless steel, and each of these materials has unique properties that suit different needs.

Sheet thicknesses are generally defined by actual thickness or using a gauge number. This is based on the material's weight, meaning that the same gauge number gives different thicknesses for different materials. Sheets come in a variety of common sizes that may have an impact on the design of your parts.

In this chapter, we introduced SolidWorks Sheet Metal and learned how to set up a Sheet Metal workspace and create Base Flanges. These are usually the first feature in a Sheet Metal part, and we covered the three different types: Single Closed Profile, Multiple Contained Closed, and Single Open Contour.

Next, we explored the four Sheet Metal properties—Thickness, Bend Radius, Bend Allowance, and Auto Relief—and how these can be edited to adjust the properties of the entire part.

Finally, we learned how 3D parts can be flattened, which is essential if they are to be made from metal sheets in the real world. On a similar note, we looked at common sheet metal materials and sheet sizes, and how these might be relevant to your final design.

In Chapter 2, Adding Bends Using Edge Flanges, we will start to build up a 3D design by learning how to use Edge Flanges to add extra detail to the Base Flange.