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Create a sheet metal component using Fusion.
Type:
Tutorial
Length:
12 min.
Transcript
00:03
In Fusion, a sheet metal part starts out as a flat piece of metal with a consistent thickness.
00:09
A flange feature consists of a face and bend connected to an existing face along an edge.
00:16
In the Design workspace, switch to the Sheet Metal toolbar.
00:20
Click the Create menu to access tools related to sheet metal creation, such as New Component, Flange, and Create Flat Pattern.
00:29
In the Modifier group, you find tools such as Unfold and Sheet Metal Rules.
00:34
To create and work with a sheet metal component, such as an outlet box, start with a blank workspace.
00:40
On the Sheet Metal toolbar, Create group, click New Component.
00:46
In the New Component dialog, the Type defaults to Sheet Metal.
00:51
Decide if the component will be an External or Internal component, then enter a name, such as “Outlet Box”.
00:58
You have the option to set the Sheet Metal Rule.
01:01
For this example, leave the default Stainless steel (in) rule selected, and then click OK.
01:08
A new component is added to the Browser, with an icon that looks like a sheet metal part.
01:14
From the Create group, click Create Sketch, then select the XZ plane.
01:20
To start drawing the first profile, on the Sketch toolbar, expand the Create menu, and select Rectangle > Center Rectangle.
01:31
Starting from the origin, create a rectangle that is 2 in by 3 in.
01:36
In the Sketch Palette, click Finish Sketch.
01:39
Now, you can use the Flange tool, which is a combination of four tools in one.
01:45
The Flange tool can be used to create a sheet metal base flange, an edge flange, a contour flange,
01:51
or a lofted flange, based on the profiles you select.
01:56
From the Create group, click Flange.
01:59
Select the profile to add thickness and create a sheet metal base flange, based on the specified sheet metal rule.
02:06
In the Flange dialog, you can specify the Orientation you want the sheet metal to extrude to: Side 1, Side 2, or Center.
02:16
For this example, select Side 1, and then click OK.
02:22
You can create a bend in this new body using edge flange.
02:26
Click Flange again and select the upper-right edge of the base flange.
02:31
Specify the Height of the bend—in this case, 2.5 in.
02:37
The bend is automatically created according to the bend rules.
02:41
You can also select multiple edges at the same time.
02:45
In the Flange dialog, click Add selection set, then select the opposite edge.
02:51
You can set other options, such as the Angle of the bend, Height Datum and Bend Position.
02:58
A sample block is shown here as a reference, to enable you to see these options more clearly.
03:03
The block is 2 in wide and 2.5 in tall.
03:08
If the Height Datum is set to Inner Faces, the 2.5 in height is measured from the inside face to the top of the part,
03:15
so it extends above the sample block.
03:18
If you select Outer Faces, the 2.5 in is measured from the outside or the bottom of the sheet metal part to the top.
03:26
With the Bend Position set to Inside, the edge flanges are inside the 2-inch width,
03:32
and with Outside selected, these areas of the part are outside of the 2-inch width.
03:37
Selecting Adjacent starts the bends adjacent to the two-inch width, and with Tangent selected, the bends are tangent to the 2-inch width.
03:47
Typically, you use Inside or Outside bend positions.
03:51
You can also Flip directions of the bend, set Miter Corners, or Override the sheet metal rules.
03:58
Click OK to accept the parameters and create the new flanges.
04:03
You can draw an open profile and turn it into a sheet metal part using a contour flange.
04:09
For this example, click Create Sketch and select the top face of the left flange.
04:14
In the Create group, click Line.
04:17
Draw an angled line that runs along the existing sheet metal part, then down and to the right, with another extension line to the right.
04:26
Click Finish Sketch.
04:29
Back on the Sheet Metal toolbar, Create group, click Flange.
04:34
Select the open profile, start to drag the height down, and then click OK.
04:40
Notice that the corners of the sheet metal part are bent accordingly.
04:44
Even though you created a sharp-edged sketch, this was created as a new body, so you can move it down if you want.
04:52
The last tool, the join flange, enables you to join sheet metal parts together, even if they are not touching.
04:58
Click Create Sketch and select the right face of the last flange you added.
05:04
In the Create group, click Line and draw an angled line that runs up and to the left with another extension line.
05:12
Click Finish Sketch.
05:14
Once again, on the Sheet Metal toolbar, Create group, click Flange.
05:20
First, click to select the new profile, then select the top edge of the open flange sheet metal part.
05:27
Click OK, and they are automatically joined together.
05:31
Again, even if your profile is not touching the sheet metal part, it will still extend and join.
05:37
This is a great way to create features, such as hems.
05:41
Now, you can add two more flanges on the other edges.
05:45
Click Flange again, select the two remaining edges on the base of the box, and drag up.
05:52
Click an existing flange to grab its height.
05:55
Make sure that the Height Datum is set to Inner Faces and the Bend Position is Inside.
06:01
Click OK.
06:03
Depending on the first set of vertical flanges, you may need to offset the side faces to provide clearance when you bend the edges.
06:10
Right-click, and from the Marking menu, select Press Pull.
06:16
Select the four faces on the side of the left and right flanges.
06:21
Set an offset of 0.03 in, then click OK.
06:26
Click Flange again.
06:28
Click the inside edge of the side flange.
06:31
Click and drag the height to about 0.5 in.
06:35
Based on the preview, you can change any settings, such as the Bend Position.
06:40
In this case, set it to Outside.
06:43
This flange will not take up the whole distance along the edge.
06:47
Select a different Edge option in the flange dialog:
06:51
Full Edge extends the full distance of the edge.
06:54
Symmetric enables you to specify a distance for the length of the flange symmetrically.
06:59
Note that the distance is half of the flange length.
07:03
Two Sides gives you the option to specify the length of the flange using two distances, such as 0.25 up and 0.75 down.
07:12
Two Offsets enables you to specify a distance from a reference point or plane.
07:17
In this example, select Symmetric, and then set the Distance value to 0.4 in.
07:24
To do the same on the other side, click Add Selection Set, then select the opposite edge.
07:31
Again, select Symmetric and enter a Distance of 0.4 in.
07:36
Add another selection set, and this time, rotate the view to select the other two edges.
07:42
Select the first edge, then press and hold Ctrl as you select the second edge.
07:48
Set the same Edge and Distance.
07:52
Once complete, click OK.
07:56
You also can create an automatic miter flange.
07:60
Click Flange again, then select the four top inner edges.
08:04
With the Miter Corners option selected in the dialog, when you drag the arrow, the corners are automatically mitered.
08:11
Click Cancel to cancel the command.
08:14
Add some symmetric flanges on the top for screw mounts.
08:18
Click Flange and select the top edges on the front and back.
08:22
Set edge 1 to Symmetric, the Distance to 0.2 in, and the Height to 0.5 in.
08:32
Set edge 2 to Symmetric and the Distance to 0.2 in.
08:37
Set the Height Datum to Inner Faces and the Bend Position to Inside.
08:44
You can override the sheet metal rules by selecting Override Rules.
08:49
Then, select Bend Relief Override, which enables you to change the Relief Shape to Straight.
08:56
Click OK.
08:57
You can also use regular modeling tools, such as Fillet, Chamfer, and Offset.
09:04
In the Modify group, click Fillet, select the corner edges on the new tabs,
09:09
and set the Radius to 0.2.
09:12
Click OK.
09:14
Use the Hole tool to add a couple of holes that reference the curved edges.
09:18
Press H to start the Hole command.
09:21
Select the top surface of one of the flanges, then select the curved edge.
09:26
Set the Hole Diameter to 0.2 in and make sure the hole cut out goes through the part by dragging the arrow.
09:34
Click OK.
09:36
Press H again, and this time, select the opposite flange face and curved edge.
09:42
Once the hole is placed, click OK.
09:45
The outlet box is mostly complete.
09:48
Now you can unfold it to see what it would look like flat.
09:52
In the Modify group, click Unfold.
09:55
Then, select a stationary entity, or the face that will stay fixed while the other bends unfold against it.
10:02
You have the option to unfold only selected bins, but in this case, select Unfold all bins to unfold the entire part.
10:11
Click OK.
10:13
You can still make changes to the sheet metal part in its unfolded state.
10:18
Create a new sketch and select the top face of the central flange.
10:22
Expand the Create menu, and select Slot > Center to Center Slot.
10:28
Draw a slot that crosses over multiple bends across the middle of the box.
10:33
Click Finish Sketch.
10:36
From the Create group, click Extrude and extrude the slot profile through the unwrapped pattern.
10:43
Click OK.
10:45
This cuts the slot through the material.
10:47
On the Sheet Metal toolbar, click Refold Faces.
10:52
When the part refolds, you can see how the slot folds with it.
Video transcript
00:03
In Fusion, a sheet metal part starts out as a flat piece of metal with a consistent thickness.
00:09
A flange feature consists of a face and bend connected to an existing face along an edge.
00:16
In the Design workspace, switch to the Sheet Metal toolbar.
00:20
Click the Create menu to access tools related to sheet metal creation, such as New Component, Flange, and Create Flat Pattern.
00:29
In the Modifier group, you find tools such as Unfold and Sheet Metal Rules.
00:34
To create and work with a sheet metal component, such as an outlet box, start with a blank workspace.
00:40
On the Sheet Metal toolbar, Create group, click New Component.
00:46
In the New Component dialog, the Type defaults to Sheet Metal.
00:51
Decide if the component will be an External or Internal component, then enter a name, such as “Outlet Box”.
00:58
You have the option to set the Sheet Metal Rule.
01:01
For this example, leave the default Stainless steel (in) rule selected, and then click OK.
01:08
A new component is added to the Browser, with an icon that looks like a sheet metal part.
01:14
From the Create group, click Create Sketch, then select the XZ plane.
01:20
To start drawing the first profile, on the Sketch toolbar, expand the Create menu, and select Rectangle > Center Rectangle.
01:31
Starting from the origin, create a rectangle that is 2 in by 3 in.
01:36
In the Sketch Palette, click Finish Sketch.
01:39
Now, you can use the Flange tool, which is a combination of four tools in one.
01:45
The Flange tool can be used to create a sheet metal base flange, an edge flange, a contour flange,
01:51
or a lofted flange, based on the profiles you select.
01:56
From the Create group, click Flange.
01:59
Select the profile to add thickness and create a sheet metal base flange, based on the specified sheet metal rule.
02:06
In the Flange dialog, you can specify the Orientation you want the sheet metal to extrude to: Side 1, Side 2, or Center.
02:16
For this example, select Side 1, and then click OK.
02:22
You can create a bend in this new body using edge flange.
02:26
Click Flange again and select the upper-right edge of the base flange.
02:31
Specify the Height of the bend—in this case, 2.5 in.
02:37
The bend is automatically created according to the bend rules.
02:41
You can also select multiple edges at the same time.
02:45
In the Flange dialog, click Add selection set, then select the opposite edge.
02:51
You can set other options, such as the Angle of the bend, Height Datum and Bend Position.
02:58
A sample block is shown here as a reference, to enable you to see these options more clearly.
03:03
The block is 2 in wide and 2.5 in tall.
03:08
If the Height Datum is set to Inner Faces, the 2.5 in height is measured from the inside face to the top of the part,
03:15
so it extends above the sample block.
03:18
If you select Outer Faces, the 2.5 in is measured from the outside or the bottom of the sheet metal part to the top.
03:26
With the Bend Position set to Inside, the edge flanges are inside the 2-inch width,
03:32
and with Outside selected, these areas of the part are outside of the 2-inch width.
03:37
Selecting Adjacent starts the bends adjacent to the two-inch width, and with Tangent selected, the bends are tangent to the 2-inch width.
03:47
Typically, you use Inside or Outside bend positions.
03:51
You can also Flip directions of the bend, set Miter Corners, or Override the sheet metal rules.
03:58
Click OK to accept the parameters and create the new flanges.
04:03
You can draw an open profile and turn it into a sheet metal part using a contour flange.
04:09
For this example, click Create Sketch and select the top face of the left flange.
04:14
In the Create group, click Line.
04:17
Draw an angled line that runs along the existing sheet metal part, then down and to the right, with another extension line to the right.
04:26
Click Finish Sketch.
04:29
Back on the Sheet Metal toolbar, Create group, click Flange.
04:34
Select the open profile, start to drag the height down, and then click OK.
04:40
Notice that the corners of the sheet metal part are bent accordingly.
04:44
Even though you created a sharp-edged sketch, this was created as a new body, so you can move it down if you want.
04:52
The last tool, the join flange, enables you to join sheet metal parts together, even if they are not touching.
04:58
Click Create Sketch and select the right face of the last flange you added.
05:04
In the Create group, click Line and draw an angled line that runs up and to the left with another extension line.
05:12
Click Finish Sketch.
05:14
Once again, on the Sheet Metal toolbar, Create group, click Flange.
05:20
First, click to select the new profile, then select the top edge of the open flange sheet metal part.
05:27
Click OK, and they are automatically joined together.
05:31
Again, even if your profile is not touching the sheet metal part, it will still extend and join.
05:37
This is a great way to create features, such as hems.
05:41
Now, you can add two more flanges on the other edges.
05:45
Click Flange again, select the two remaining edges on the base of the box, and drag up.
05:52
Click an existing flange to grab its height.
05:55
Make sure that the Height Datum is set to Inner Faces and the Bend Position is Inside.
06:01
Click OK.
06:03
Depending on the first set of vertical flanges, you may need to offset the side faces to provide clearance when you bend the edges.
06:10
Right-click, and from the Marking menu, select Press Pull.
06:16
Select the four faces on the side of the left and right flanges.
06:21
Set an offset of 0.03 in, then click OK.
06:26
Click Flange again.
06:28
Click the inside edge of the side flange.
06:31
Click and drag the height to about 0.5 in.
06:35
Based on the preview, you can change any settings, such as the Bend Position.
06:40
In this case, set it to Outside.
06:43
This flange will not take up the whole distance along the edge.
06:47
Select a different Edge option in the flange dialog:
06:51
Full Edge extends the full distance of the edge.
06:54
Symmetric enables you to specify a distance for the length of the flange symmetrically.
06:59
Note that the distance is half of the flange length.
07:03
Two Sides gives you the option to specify the length of the flange using two distances, such as 0.25 up and 0.75 down.
07:12
Two Offsets enables you to specify a distance from a reference point or plane.
07:17
In this example, select Symmetric, and then set the Distance value to 0.4 in.
07:24
To do the same on the other side, click Add Selection Set, then select the opposite edge.
07:31
Again, select Symmetric and enter a Distance of 0.4 in.
07:36
Add another selection set, and this time, rotate the view to select the other two edges.
07:42
Select the first edge, then press and hold Ctrl as you select the second edge.
07:48
Set the same Edge and Distance.
07:52
Once complete, click OK.
07:56
You also can create an automatic miter flange.
07:60
Click Flange again, then select the four top inner edges.
08:04
With the Miter Corners option selected in the dialog, when you drag the arrow, the corners are automatically mitered.
08:11
Click Cancel to cancel the command.
08:14
Add some symmetric flanges on the top for screw mounts.
08:18
Click Flange and select the top edges on the front and back.
08:22
Set edge 1 to Symmetric, the Distance to 0.2 in, and the Height to 0.5 in.
08:32
Set edge 2 to Symmetric and the Distance to 0.2 in.
08:37
Set the Height Datum to Inner Faces and the Bend Position to Inside.
08:44
You can override the sheet metal rules by selecting Override Rules.
08:49
Then, select Bend Relief Override, which enables you to change the Relief Shape to Straight.
08:56
Click OK.
08:57
You can also use regular modeling tools, such as Fillet, Chamfer, and Offset.
09:04
In the Modify group, click Fillet, select the corner edges on the new tabs,
09:09
and set the Radius to 0.2.
09:12
Click OK.
09:14
Use the Hole tool to add a couple of holes that reference the curved edges.
09:18
Press H to start the Hole command.
09:21
Select the top surface of one of the flanges, then select the curved edge.
09:26
Set the Hole Diameter to 0.2 in and make sure the hole cut out goes through the part by dragging the arrow.
09:34
Click OK.
09:36
Press H again, and this time, select the opposite flange face and curved edge.
09:42
Once the hole is placed, click OK.
09:45
The outlet box is mostly complete.
09:48
Now you can unfold it to see what it would look like flat.
09:52
In the Modify group, click Unfold.
09:55
Then, select a stationary entity, or the face that will stay fixed while the other bends unfold against it.
10:02
You have the option to unfold only selected bins, but in this case, select Unfold all bins to unfold the entire part.
10:11
Click OK.
10:13
You can still make changes to the sheet metal part in its unfolded state.
10:18
Create a new sketch and select the top face of the central flange.
10:22
Expand the Create menu, and select Slot > Center to Center Slot.
10:28
Draw a slot that crosses over multiple bends across the middle of the box.
10:33
Click Finish Sketch.
10:36
From the Create group, click Extrude and extrude the slot profile through the unwrapped pattern.
10:43
Click OK.
10:45
This cuts the slot through the material.
10:47
On the Sheet Metal toolbar, click Refold Faces.
10:52
When the part refolds, you can see how the slot folds with it.
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