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The specific formulas for finding these numbers are not as important as an intuitive grasp of what
the numbers mean and how they are used, at least in relation to using SolidWorks to model sheet
metal parts. The numbers used to fill out Bend Tables using K, BA, or BD values are typically taken
from experimentally developed tables.
Auto Relief
Auto reliefs were formerly called Bend reliefs. You can specify three different Auto relief options to
be applied automatically to bends that end in the middle of material. These options are illustrated
in Figure 29.7.
FIGURE 29.7
The three Auto relief configurations: Rectangular, Tear, and Obround
Rectangular Tear Obround
For the Rectangular and Obround types, you can control the width and the distance past the tan-
gent line of the bend through the Relief Ratio selection box, which is immediately below the type
selection box in the Sheet Metal PropertyManager. This ratio is the width of the relief divided by
the part thickness. For the Rectangular relief, a ratio of .5 and a thickness of .050 inches means
that the relief is .025 inches wide and that it goes .025 inches deeper into the part beyond the tan-
gent line of the bend. The Obround relief goes slightly deeper because it has a full radius after the
distance past the tangent line of the bend, and so it essentially goes a total of one full material
thickness past the tangent line.
The Tear relief is simply a face-to-face shear of the material with no gap.
Flat Pattern feature
The Flat Pattern feature is added automatically to the end of the tree when the Base Flange feature
is added. This feature is used to flatten the sheet metal part when the feature is unsuppressed. The
Flatten toolbar button acts as a toggle to unsuppress or suppress the Flat Pattern feature in the tree.
It may be a little confusing, but the Flatten toolbar button and the flat-pattern feature in the
FeatureManager refer to the same functionality. As mentioned earlier, the Flat Pattern has a couple
Chapter 29: Using SolidWorks Sheet Metal Tools
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of special properties that are not seen in other features. The first is that it remains at the bottom of
the FeatureManager when other Sheet Metal features are added.
The second property of the Flat Pattern feature is that it is added in the suppressed state. When it is
unsuppressed, it flattens out the sheet metal bends.
By editing the Flat Pattern feature, you can set a few options. The Flat Pattern PropertyManager is
shown in Figure 29.8.
FIGURE 29.8
The Flat Pattern PropertyManager
The Fixed face parameter determines which face remains stationary when the part is flattened out.
Generally, the largest face available is selected automatically, but if you want to specify a different
face to remain stationary, you can do that here.
When the Merge faces option is selected, it causes the Flat Pattern to form a single face rather than
being broken up by the tangent lines around the bends. This does a few things. First, selecting the
face of the flattened part and clicking Convert Entities (found on the Sketch toolbar) makes an out-
line of the entire flattened part, which is easier to use for certain programming applications.
Second, the edges around the outside are not broken up. Third, the tangent edges around the
bends are not shown. The differences between Flat Patterns with this option selected and
unselected are shown in Figure 29.9.
Bend lines are shown in both examples in Figure 29.9.
When you turn select the Simplify Bends option, it simplifies curved edges that are caused by flat-
tening bends to straight lines from arcs or splines. When the option is unselected, the complex
edges remain complex. Simple edges can be cut by standard punches, and do not require
Computer Numerical Control (CNC) controlled lasers or abrasive water jets.
The Corner Treatment option controls whether or not a corner treatment is applied to the Flat
Pattern of a part. The corner treatment is illustrated in Figure 29.10. The model used to create this
corner used a Miter Flange around the edges of a rectangular sheet.
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FIGURE 29.9
The Merge Faces option showing on (selected) and off (unselected)

Merge faces on Merge faces off
FIGURE 29.10
Using the Corner Treatment setting in the Flat Pattern PropertyManager
Corner treatment on
Corner treatment off
Chapter 29: Using SolidWorks Sheet Metal Tools
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Note
You can export a *.dxf file of the Flat Pattern directly from the model without creating a drawing.
n
Edge Flange feature
The Edge Flange feature is very flexible and can be changed in several ways. If you have not kept
up with the changes to Edge Flange for the last couple of releases, then you may find some
surprises.
Edge Flange is intended to turn a 90-degree flange from a selected straight edge in the direction
and distance specified using the default thickness for the part. The default process for this feature
is that you select the tool, select the edge, and then drag the distance, clicking a distance reference
such as a vertex at the end of another flange of equal length or typing a distance value manually.
You can select multiple edges from a part that do not necessarily need to touch one another. That
is all there is to a simple default flange, although several options give you some additional options
for angle, length, and so on. Figure 29.11 shows the Edge Flange PropertyManager, as well as a
simple flange.
FIGURE 29.11
The Edge Flange PropertyManager and a simple flange
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Edit Flange Profile
The Edit Flange Profile button in the Edge Flange PropertyManager enables you to edit a sketch to
shape the flange in some way other than rectangular, or to otherwise edit the shape of the flange.
Notice in Figure 29.11 that both of the flanges made by a singe flange feature have been edited.

You can do this by selecting the flange for which you want to edit the profile before clicking the
Edit Flange Profile button.
Note
If you have added dimensions to the sketch, as shown in Figure 29.11, then you will no longer be able to use
the arrow to drag the length of the flange. To edit the length, you will need to edit the sketch or double-click
the feature, and then double-click the dimensions that you want to change.
n
You can add holes to the flange profile as nested loops. This enables you to avoid creating addi-
tional hole features, but does not enable you to control suppression state independently from the
flange feature.
You can make flanges go only part of the way along an edge by pulling one of the end lines back
from the edge. This works even though the end lines appear black and fully defined. A situation
where the sketch has been edited this way is shown in the image to the right in Figure 29.11.
Use default radius
This option enables you to override the default inside bend radius that is set for the entire part for
this feature. The bend radii for individual bends within an Edge Flange that has multiple flanges
cannot be set; the only override is at the feature level. If you need individual bends to have differ-
ent bend radii, then you need to do this using multiple Edge Flange features.
Gap distance
The gap distance is illustrated in Figure 29.12. The Gap Distance selection box is only active when
you have selected multiple edges in the main selection box for this feature. The gap refers to the
space between the inside corners of the perpendicular flanges.
Angle
Because the Edge Flange is not dependent on a sketch for its angle like the Base Flange is, you can
set the angle in the Angle panel of the PropertyManager. The values that this selection box can
accept range from any value larger than zero to any value smaller than 180. Of course, each flange
has practical limits. In the flange shown in Figure 29.13, the limitation is reached when the bend
radius runs into the rectangular notch in the middle of the flange to the right, at about 158
degrees. The angle affects all the flanges that are made with the feature. To create a situation where
different flanges have different angles, you need to create separate flange features.

Chapter 29: Using SolidWorks Sheet Metal Tools
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FIGURE 29.12
Specifying the gap distance
Gap
FIGURE 29.13
Establishing the limit of the flange angle
Flange Length
As mentioned earlier, if you have edited the Flange Profile sketch and a flange length dimension is
applied in the sketch, then the flange length is taken from that sketch dimension. If this dimension
has not been added to the profile sketch, then the options for this setting in the PropertyManager
Flange Length panel are Blind and Up To Vertex. Using Up To Vertex is a nice way to link the
lengths of several flanges.
Flange Position
The small icons for Flange Position should be fairly self-explanatory, with the dotted lines indicat-
ing the existing end of the material. The names for these options, in order from left to right, are
l
Material Inside
l
Material Outside
l
Bend Outside
l
Bend From Virtual Sharp (for use when an angle is involved)
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906
Trim side bends
In situations where a new flange is created next to an existing flange, and a relief must be made in
the existing flange to accommodate the new flange, you can select the Trim side bends option to
trim back the existing flange. Leaving this option unselected simply creates a relief cut, as shown in

Figure 29.14. This is functionality that requires some imagination from the user. A real sheet metal
part manufactured like this would have an area at the corner where the deformation from the
bends in different directions overlaps. This overlapping bend geometry is too complex for
SolidWorks to create automatically, so it offers you a couple of options for how you would like to
visually represent the corner. The Flat Pattern is correct, but the formed model requires some
imagination.
FIGURE 29.14
Using the Trim side bends option
Trim Side Bends off Trim Side Bends on
Curved edges
Edge Flanges can be created on curved edges, but the curved edge must be on a planar face. For
example, if the part were the top of a mailbox, then an Edge Flange could not be put on the curve
on the top of the mailbox. The flange would have to be made as a part of the flat end of the mail-
box, instead.
Figure 29.15 shows Edge Flanges used on a part. Notice that reliefs are added to the ends of the
bends, although they are not really needed.
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FIGURE 29.15
Curved Edge Flanges on a part
Notice bend reliefs where they are not needed
All the edges that you select to be used with a curved Edge Flange must be tangent. This means
that in Figure 29.15, neither of the Edge Flanges could have been extended around the ends of the
part. You would need to create separate Edge Flange features for those edges.
Because these Edge Flanges are made in such a way that they are developable surfaces, they can be
(and are) flattened in such a way that they do not stretch the material of the flange when the flat is
compared to the formed shape. Doubtless there is some deformation in between the two states in
the actual forming of this flange, and so its manufacturing accuracy may not be completely reliable.
Miter Flange feature
The Miter Flange feature can create picture frame–like miters around corners of parts, and cor-

rectly recognizes the difference between mitered inside corners and mitered outside corners. The
PropertyManager and a sample Miter Flange are shown in Figure 29.16.
A Miter Flange feature starts off with a sketch that is perpendicular to the starting edge of the Miter
Flange feature.
Tip
A quick way to start a sketch for a Miter Flange that is on a plane perpendicular to a selected edge is to select
the edge, and then click a sketch tool. This automatically creates a plane perpendicular to the edge at the near-
est endpoint.
n
Miter Flange sketches can have single lines or multiple lines. They can even have arcs. Still,
remember that just because you can make it in SolidWorks does not mean that the manufacturer
can make it. It is often a good idea to check with the manufacturer to ensure that the part can be
made. Also, you usually learn something from the experience.
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FIGURE 29.16
The Miter Flange PropertyManager and a sample part
Tip
When selecting edges for the Miter Flange to go on, be sure to remain consistent in your selection. If you start
by selecting an edge on the top of the part, then you should continue selecting edges on the top of the part. If
you do not, then SolidWorks prompts you with a warning message in a tool tip that says that the edge is on the
wrong face.
n
Some of the controls in the Miter Flange PropertyManager should be familiar by now, such as Use
default radius, Flange Position, Trim side bends, and Gap Distance. You have seen these controls
before in the Edge Flange PropertyManager.
The Start/End Offset panel enables you to pull a Miter Flange back from an edge without using a
cut. If you need an intermittent flange, then you may need to use cuts or multiple Miter Flange fea-
tures, as shown in Figure 29.17.
Hem feature

The Hem feature is used to roll over the edge of a sheet metal part. This feature is often used to
smooth over a sharp edge or to add strength to the edge. You can also use it for other purposes,
such as to capture a pin for a hinge. SolidWorks offers four different hem styles — Closed, Open,
Tear Drop, and Rolled — which are shown as icons on the Hem PropertyManager. The
PropertyManager for the Hem feature is shown in Figure 29.18.
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FIGURE 29.17
The Start/End Offset settings for a Miter Flange
End Offset
Start Offset
Sketch for
Miter Flange
FIGURE 29.18
The Hem PropertyManager and a sample hem
One of the limitations to keep in mind with regard to hems is that SolidWorks cannot fold over a
part so that the faces touch perfectly line on line. Doing this would cause the two sections of the
part to merge into a larger piece, thus removing the coincident faces. SolidWorks, computers, and
mathematics in general do not always handle the number zero very well. In reality, you can often
see light through these hems, and so a perfectly flush hem may not be as accurate as it seems.
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910
You can edit the profile of the Hem, like an Edge Flange, to control the length of the edge that is
hemmed. To do this, click the Edit Hem Width button below the Edges selection box in the Hem
PropertyManager, shown in Figure 29.18.
Jog feature
The Jog feature puts a pair of opposing bends on a flange so that the end of the flange is parallel to,
but offset from, the face where the jog started. The Jog PropertyManager and a sample jog are
shown in Figure 29.19.
FIGURE 29.19

The Jog PropertyManager and a sample jog
The Jog feature is created from a single sketch line on the face of a sheet metal part. The geometry
to be jogged should not have any side bends; it should be a simple tab-like flange, as shown in
Figure 29.19. The line to create the jog can be drawn at an angle, causing the jog to also be angled.
The three icons on the Jog Offset panel illustrate what dimension is being controlled by that setting.
Fixed Face
Like most sheet metal features, the Jog feature bends faces on the part, and when it does so,
although it may be obvious to you as the user, it is not obvious to the software which face should
remain stationary and which faces should be moved by the bend. The Fixed Face selection box
enables you to select a face, or in this case, a part of a face, that you want to remain stationary as
the rest of the faces move. The black dot on the face identifies it as stationary.
Chapter 29: Using SolidWorks Sheet Metal Tools
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Tip
Problems can sometimes arise when you are using configurations that change sizes, because these markers for
fixed faces can be pushed onto other faces. This can cause problems with assemblies and drawings, and in gen-
eral makes visualization difficult. In cases like this, it may be advisable to select a larger face or one that has
fewer changes, if possible, to be used as the fixed face.
n
Jog Offset
You can control the direction of the jog by using the arrow button to the left of the end condition
selection box. You can control the jog distance by selecting the end conditions Up To Surface, Up
To Vertex, or Offset From Surface. The default setting is Blind, in which you simply enter a dis-
tance for the offset, in exactly the same way that end conditions are controlled for features such as
extrudes.
Fix projected length
One setting that may not be obvious is the Fix projected length. This refers to the length of the
flange that the jog is altering. In Figure 29.19, you can see that the height of the jogged feature is
the same as the height of the original feature. The jog obviously requires more material than the
original, but the Fix projected length option is selected, and so the height is maintained. If you

deselected this option, then the finished height of the flange after the jog is added would be
shorter, because the material is used by the jog and additional material would not be added. For
comparison, the image to the right in Figure 29.19 shows this situation.
Jog Position
The Jog Position selection establishes the relationship between the sketched line and the first bend
tangent line. The Jog Position icons have tool tips with the following names, from left to right:
Bend Centerline, Material Inside, Material Outside, and Bend Outside.
Jog Angle
The Jog Angle enables you to change the angle of the short perpendicular section of the jog. You
can angle it to smooth out the jog (angles of less than 90 degrees) or to curl back on itself (angles
of more than 90 degrees). Again, be careful to check with your manufacturer’s capabilities.
Sketched Bend feature
Sketched Bend works in some respects like half of a jog. It requires the sketch line and the Fixed
Face selection. You define a bend position with the same set of icons that you used in the jog, and
you assign a bend angle in the same way.
Tip
You can use the Sketched Bend feature to dog ear corners. You do this by drawing a line across the corner at
an angle and setting the angle to 180 degrees and then overriding the default radius with a much smaller one,
such as .001 inches.
n
Unlike Jog, the Sketched Bend feature does not show you a preview. The Sketched Bend
PropertyManager is shown in Figure 29.20.
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FIGURE 29.20
The Sketched Bend PropertyManager
Closed Corner feature
The Closed Corner feature extends flanges on the sides to meet with other flanges. It is typically
used when corners leave big open gaps in order to create a corner that is more easily welded shut
(although welds cannot be created in sheet metal parts in SolidWorks). Figure 29.21 shows a part

where angled flanges have been applied. This creates big gaps in the corners. Although a Miter
Flange may have been better, these were created using regular Edge Flanges.
FIGURE 29.21
Applying the Closed Corner feature
Faces to Extend
You must select the thickness face of one of the flanges in order to extend it. Selecting one face
automatically selects the matching face from the other flange that you also want to extend. The
Corner Type selection icons depict the selected face as red, and the three icons display tooltips:
Butt, Overlap, and Underlap.
Chapter 29: Using SolidWorks Sheet Metal Tools
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Faces to Match
The faces selected in the Faces to Match selection box act as an “up to” end condition for the faces
to extend. Prior to SolidWorks 2010, the Closed Corner feature always automatically selected a
matching face to extend for each face selected, when appropriate. SolidWorks 2010 enables you to
manually select matching faces in the Faces to Match selection box for those times when the auto-
matic selection does not work.
Note
If you deselect faces in either the Faces to Extend or Faces to Match selection boxes, the Auto Propagation
option toggles off to enable you to make selections manually.
n
Gap
The Gap setting enables you to specify how close you want the closed corner to be. Keep in mind
that you cannot use the number zero in this field. If you do, then SolidWorks reminds you to
“Please enter a number greater than or equal to 0.00003937 and less than or equal to
0.86388126.” It is good to know your limits.
Overlap/Underlap ratio
The Overlap/Underlap ratio setting controls how far across the overlapped face the overlapping
flange reaches. Full overlap is a ratio of 1, and a Butt condition is (roughly) a ratio of zero. This
ratio is only available when you have specified Overlap or Underlap for the corner type.

Open bend region
The Open bend region option affects how the finished corner looks in the bend area. If Open bend
region is selected, then a small gap is created at the end of the bend. If the option is deslected, then
SolidWorks fills this area with geometry. Figure 29.22 shows the finished model with this option
selected and unselected, as well as the resulting Flat Patterns for each setting.
FIGURE 29.22
The Open bend region option, both selected and unselected, and the resulting Flat Patterns
Open Bend
Region on
Open Bend
Region on –
flat pattern
Open Bend
Region off
Open Bend
Region off –
flat pattern
Part VII: Working with Specialized Functionality
914
Coplanar faces
When the Coplanar option is selected, any faces that are coplanar with any selected faces are also
selected Corner Trim and Break Corner features. The Corner Trim feature is available only when
the sheet metal part is in its flattened state. The Corner Trim PropertyManager also has the Break
Corner Options interface built right into it. However, the Break Corner feature is only available
when the sheet metal part is in its folded state. Figure 29.23 shows the combined interface. Both
functions are included here, and SolidWorks treats them as if they are part of a single function.
FIGURE 29.23
The Corner Trim PropertyManager, including the Break Corner Options panel
When finished, the Corner Trim feature places itself after the Flat Pattern feature in the
FeatureManager. It similarly follows the suppress/unsuppress state of the Flat Pattern feature.

When the Break Corner feature is used on its own, it is placed before the Flat Pattern feature. With
this in mind, it seems best to use Break Corner as a separate feature unless it is being used specifi-
cally to alter the Flat Pattern in a way that cannot be done from the folded state.
Break Corner on its own is primarily used to remove sharp corners using either a chamfer or a
rounded corner. This tool is set up to filter edges on the thickness of sheet metal parts, which is
useful, because these edges are otherwise difficult to select without a lot of zooming. Break Corner
can also break interior corners.
One of the main functions of the Corner Trim feature is to apply bend relief geometry to the Flat
Pattern. The three available options are Circular, Square, and Bend Waist. These options are shown
in Figure 29.24.
Chapter 29: Using SolidWorks Sheet Metal Tools
915
FIGURE 29.24
Applying the Corner Trim Relief options
Forming Tool feature
Forming tools in SolidWorks enable you to place features that are not formed on a brake press.
These are features that are not straight-line bends, but rather punched, drawn, formed, lanced,
sheared, or otherwise deformed material.
One of the important things to understand about forming tools is that they do not stretch the
material in the SolidWorks part in the same way that happens in a real-life forming operation. In
real life, material is thinned when it is punched, stamped, or drawn. In SolidWorks, the thickness
of a sheet metal part remains the same, regardless of what happens to it. For this reason, you need
to be careful when using mass properties of sheet metal parts or doing stress analysis of parts that
have formed features. You might consider taking your part weight from the Flat Pattern rather than
from the formed sheet metal.
SolidWorks installs with a library of fairly simple forming tools that you can use as a starting point
for your own personal customized library. You can also examine some of these tools to see how
they create particular effects. You find this library in your Design Library in the Task pane. Some of
the more interesting forming tools are the lances and louvers.
Creating forming tools

Forming tools are essentially a part that is used as a tool to form another part. One flat face of the
forming tool part is designated as a Stopping Face, which is placed flush with the top face of the
sheet metal part. You can move and rotate the tool with the Modify Sketch tool, and you can use
dimensions or sketch relations to locate it.
Creating forming tools is far easier than it used to be. This section of the chapter gives you the
information that you need to effectively create useful forming tools, addresses the limitations and
unintended uses of forming tools, and provides a couple of hints for more complex forming tool
creation.
To create a forming tool, click the Forming Tool button on the Sheet Metal toolbar. Figure 29.25
shows the PropertyManager interface for this tool.
Part VII: Working with Specialized Functionality
916
FIGURE 29.25
The Form Tool PropertyManager and a sample tool with orientation sketch
The Stopping Face turns a special color, and so do any faces that are selected in the Faces to
Remove selection box. Faces to Remove means that those faces will be cutouts in the sheet metal
part.
Another aspect of the forming tool is the orientation sketch. Create the orientation sketch by using
Convert Entities on the Stopping Face. If you have used this function in any of its previous ver-
sions, then you know that this latest iteration is far easier to create than before. However, to me, it
looks like the orientation sketch has taken a step backward. The orientation sketch cannot be man-
ually edited, and so for forming tools where footprints are symmetrical, but other features in the
tool are not, you cannot tell from the sketch which direction the forming tool should face.
Orientation could be managed more easily in earlier versions of forming tools because the place-
ment sketch was just a manually created sketch.
When creating a forming tool, you must remember to build in generous draft and fillets, and not to
build undercuts into the tool. Also keep in mind that when you have a concave fillet face on the
tool, the radius becomes smaller by the thickness of the sheet metal; as a result, you must be care-
ful about minimum radius values on forming tools. If there is a concave face on the tool that has a
.060-inch radius and the tool is applied to a part with a .060-inch thickness, then the tool will

cause an error because it forms a zero radius fillet, which is not allowed. Errors in applied forming
tool features cannot be edited or repaired, except by changing forming tool dimensions.
Once the forming tool is created, special colors are used for every face on the part. For example,
the Stopping Face is a light blue color, Faces to Remove are red, and all the other faces are yellow.
Figure 29.26 shows the small addition that is made to the FeatureManager when you make a part
into a forming tool. This feature did not exist in older versions of the tool.
Forming Tool Library
The folder that the forming tools are placed into in the Design Library must be designated as a
Forming Tool folder. To do this, right-click the folder that contains the forming tools and select
Forming Tool Folder (a check mark appears next to this option).
Chapter 29: Using SolidWorks Sheet Metal Tools
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FIGURE 29.26
The FeatureManager of a forming tool part
Placing a forming tool
To place a forming tool on a sheet metal part (forming tools are only allowed to be used on parts
with sheet metal features), you can drag the tool from the library and drop it on the face of the
sheet metal part. Forming tools are limited to being used on flat faces.
From there, you can use the Modify Sketch tool or horizontal and vertical sketch relations to move
and rotate the forming tool. It may be difficult to orient it properly without first placing it, seeing
what orientation it ends up in, and then reorienting it if necessary because of the limitation men-
tioned earlier with not being able to edit the orientation sketch to give it some sort of direction
identifier.
Configurations cannot be used with forming tools like they can with library features, although you
can change dimensions by double-clicking the Forming Tool icon in the sheet metal part
FeatureManager. Forming tools are suppressed when the part is flattened.
Special techniques with forming tools
One application of forming tools that is asked for frequently is the cross break to stiffen a large, flat
sheet metal face. SolidWorks has a cosmetic cross break which I discuss next. Cross breaks are
clearly not something that SolidWorks can do using straight bends, but a forming tool can do it.

You can create the forming tool by lofting a rectangle to a sketch point on a plane slightly offset
from the plane of the rectangle. This creates a shallow pyramid shape. Open the part from the
material on the CD-ROM for Chapter 29 called
Chapter 29 – Cross Break Sheet Metal.
sldprt
to examine how this part was made. Figure 29.27 shows the Cross Break forming tool
applied to a sheet metal part.
Cross Breaks
Using a forming tool to create a cross break is overkill for most situations. You may need to do it if
you need to actually show the indented geometry. The Cross Break feature is essentially a cosmetic
cross break, and it enables you to specify the radius, angle, and direction used to create the cross
break. It does not actually change the part geometry at all, but it does add two curve-like display
entities.
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918
FIGURE 29.27
The Cross Break forming tool applied to a part
When you place a Cross Break feature, you have the option to edit the sketch profile that creates
the cross. This sketch has two intersecting lines. You cannot add more lines; the feature will fail if
you have more than two lines in the sketch. (For example, if you wanted to put three breaks across
a hexagonal face, the software will not allow this.) The lines do not have to end at a corner, but
they do have to end at an edge. If the lines extend past or fall short of an edge, the feature will dis-
play a red X error icon, but it still creates the break lines where the sketch lines are.
Figure 29.28 shows the Cross Break PropertyManager and a part to which a Cross Break was applied.
Notice that you can see the break lines through the solid, much like curves or cosmetic threads.
The Cross Break feature shows up in the FeatureManager just like any other feature, not like a cos-
metic thread, which is the only other entity in the software that the Cross Break much resembles.
FIGURE 29.28
Creating a Cross Break
Chapter 29: Using SolidWorks Sheet Metal Tools

919
Form across bends
A second special technique is a gusset or a form that goes across bends. This can be adapted in
many ways, but it is shown here going across two bends. I cannot confirm the practicality of actu-
ally manufacturing something like this, but I have seen it done.
The technique used here is to call the single long flat face of the forming tool the Stopping Face.
The vertical faces on the ends and the fillet faces must be selected in the Faces to Remove selection
box. The fillets of the outside of the forming tool also have to match the bends of the sheet metal
part exactly. You may need to edit this part each time you use it, unless you apply it to parts with
bends of the same size and separated by the same distance.
When you place the tool on the sheet metal part, you must place it accurately from side to side to
get everything to work out properly. This part is in the same location as the Cross Break file, and is
called
Chapter 29 – Form Across Bends Sheet Metal.sldprt. Figure 29.29 shows the
tool and a part to which it has been applied.
FIGURE 29.29
Forming across bends
Faces to remove (both ends)
Stopping face
Part VII: Working with Specialized Functionality
920
Lofted Bends feature
The Lofted Bends feature enables you to create transitions between two profiles. The range of func-
tionality available through the Loft feature is not available with Lofted Bends; it is limited to two
profiles with no end conditions or guide curves. Both profiles also need to be open contours in
order to allow the sheet metal to unfold.
Lofted Bends is not part of the Base Flange method, but it is part of the newer set of sheet metal
tools available in SolidWorks. Figure 29.30 shows what is probably the most common application
of this feature. The bend lines shown must be established in the PropertyManager when you create
or edit the feature. Bend Lines are only an option if both profiles have the same number of straight

lines. For example, if one of the profiles is a circle instead of a rectangle with very large fillets, then
the Bend Lines options are not available in the PropertyManager.
FIGURE 29.30
The Lofted Bends PropertyManager, a sample, and a Flat Pattern with bend lines
Chapter 29: Using SolidWorks Sheet Metal Tools
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Like the forming tools, you can also use Lofted Bends in situations for which they were probably
not intended. Figure 29.31 shows how lofting between 3D curves can also create shapes that can
be flattened in SolidWorks. In this case, a couple of intermediate steps were required to get to the
3D curves, which involve surface features.
Note
This part is included on the CD-ROM with the name Chapter 29 – wrap.sldprt.
FIGURE 29.31
Using 3D curves with Lofted Bends to create flatten complex shapes
Unfold and Fold features
Unfold is a feature that unfolds selected bends temporarily. It is typically used in conjunction with
a Fold feature to re-fold the bends. This combination is used to apply a feature that must be
applied to the Flat Pattern; for example, a hole that spans across a bend.
Figure 29.32 shows the FeatureManager of a part where this combination has been applied, as well
as the part itself, showing the bend across a hole, and the PropertyManager, which is the same for
both features.
Both the Unfold and Fold features make it easy to select the bends without zooming in, even for
small bends. A filter is placed on the cursor when the command is active, which allows only bends
to be selected. The Collect All Bends option also becomes available. This feature also requires that
you select a stationary face to hold still while the rest of the model moves during the unfolding and
folding process.
Part VII: Working with Specialized Functionality
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FIGURE 29.32
Applying the Unfold and Fold features

Making Sheet Metal Parts from
Generic Models
SolidWorks can also convert generic constant thickness models into sheet metal parts that flatten,
and on which any of the dedicated sheet metal features can be used. You can make models from
thin feature extrudes or regular extrudes with Shell features, and then use the Insert Bends feature
to make them sheet metal parts. The structure of parts created with the Insert Bends feature is
somewhat different. Figure 29.33 shows a comparison of the two methods’ FeatureManagers for
simple parts.
The most notable difference is that the Insert Bends part starts off with non-sheet metal features.
The Rip feature also stands out, but the Rip feature is not exclusive to sheet metal. Although you
can use Rip on any model, it is found only on the Sheet Metal toolbar.
The Sheet Metal feature is found in both the Base Flange and Insert Bends methods, and has the
same PropertyManager function in both methods.
The new features in the Insert Bends method are the Flatten Bends and Process Bends features. The
way the Insert Bends method works is that the model that is built with the sharp-cornered non-
sheet metal feature is flattened by the Flatten Bends feature. The model is then reconstructed with
bends by the Process Bends feature.
The main rule that SolidWorks enforces on sheet metal models regardless of how they came to be
sheet metal is that the parts should have a consistent wall thickness. When all the geometry is
made from the beginning as a sheet metal part (using the Base Flange method), there is never a
problem with this. However, when the part is modeled from thin features, cuts, shells, and so on,
there is no telling what may happen to the model.
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FIGURE 29.33
A comparison between default features for Base Flange and Insert Bends
If you perform an Insert Bends operation on a model that does not have a consistent wall thick-
ness, then the Flatten Bends and Process Bends features fail. If a thickness face is not perpendicular
to the main face of the part, then the software simply forces the situation, making the face perpen-
dicular to the main face.

Normal cut feature
If a Cut feature is placed before the Sheet Metal feature, then as far as SolidWorks is concerned, the
part is not a sheet metal part. However, if the cut feature is created after the Sheet Metal feature,
then the model has to follow a different set of rules. The “normal shear” mentioned previously is
one of those rules. In Figure 29.2, the sketch for a cut is on a plane that is not perpendicular to the
face that the cut is going into. Under a normal modeling situation, the cut just goes through the
part at an angle. However, in SolidWorks sheet metal, a new option is added to the
PropertyManager for the cut. This is the Normal cut option, and it is selected by default. You could
be modeling and never even notice this option, but it is important because it affects the geometri-
cal results of the feature.
As shown in Figure 29.34, when the Normal cut option is selected, the thickness faces of the cut
are turned perpendicular (or normal) to the face of the sheet metal. This is also important because
if the angle between the angled face and the sketch changes, the geometry of the cutout can also
change. This setting becomes more important as the material becomes thicker and as the angle
between the sketch and the sheet metal face becomes shallower.
SolidWorks allows you to have angled faces on side edges, and will maintain the angle when it flat-
tens the part. In previous versions, angles on side faces cause the Flat Pattern feature to fail. Even a