An introduction to the sketching user interface, how to create basic shapes and a base profile, and an introduction to the modify tools.
Transcript
00:03
In Fusion, sketches are the underlying geometry that support the creation of 3D solid, surface, and T-Spline bodies in your design.
00:12
To access the sketch environment, in the Solid toolbar, Create group, click Create Sketch.
00:20
On the canvas, select the initial plane or face to begin the sketch on.
00:25
In this example, the XZ plane is selected, and the environment automatically aligns to this plane.
00:32
You can disable this in the Design Preferences by deselecting the Auto look at sketch checkbox.
00:38
Back in the sketch environment, notice that you now see the Sketch toolbar, indicated by the currently active Sketch tab.
00:46
From here, you have access to sketching features and tools that follow a typical sketching
00:52
workflow—first, you create your base outline shape, before modifying it, until finally constraining it.
00:59
The first section, the Create group, is where you can find basic shapes including lines, circles, and text to create your base sketch.
01:08
Other Create commands and tools include the Mirror and Pattern commands, the Project command, and the dimensioning tool.
01:16
Once you have a base sketch in place, you can use the tools in the Modify group, such as Fillet, Trim, or Offset.
01:24
Then, use the tools in the Constraints group to maintain complete control over your design and avoid unwanted errors.
01:32
The Sketch Palette also offers additional sketch tools to help with your workflow.
01:37
After this quick run through of the sketching UI, you are ready to create some basic shapes.
01:43
Start by creating a simple line.
01:46
In the Sketch toolbar, Create group, click the Line command.
01:51
You can also press the keyboard shortcut L for line, press S to search for a command,
01:57
or right-click the canvas to access the command from the Marking menu.
02:02
Once the command has been selected, you are prompted to place the first point.
02:07
You can place the first point anywhere on the canvas.
02:11
Here, use the origin as your starting point by hovering near to it, waiting for it to snap, then clicking to place.
02:18
Once placed, drag this line away from the origin.
02:22
You can see a preview of the line, as well as two dialog boxes that let you define the length and angle, if already known.
02:30
Also, if you drag this line to the X or Z axis, it snaps to the respective axis.
02:36
Both dialog boxes and automatic snapping provide quick ways to apply constraints and dimensions to your sketch.
02:44
Create a line that does not snap to the horizontal or vertical at any length and angle by clicking once you have your position.
02:51
After you place a second point, you can drag the line out to continue and create more lines.
02:57
Notice how you can also snap to other sketch features, such as a midpoint, or by creating a perpendicular line.
03:05
To leave this as a single line for now, click the green check mark to confirm.
03:10
You are still in the Create Line mode.
03:13
To end it, press Esc or Enter on your keyboard.
03:17
At the moment, this sketch is not fully defined, meaning you can move it around and change its length simply by dragging its end point.
03:25
As you snapped to and selected the origin for the starting position,
03:29
an automatic constraint was placed, meaning this start point is locked in place.
03:34
As such, you cannot move it as you have just done with the end point.
03:39
Click this start point to see the relative constraint symbol.
03:43
If you delete this to remove the constraint, the sketched line is now free to move.
03:49
To reset the constraint, simply drag the end point back to the origin and release the mouse button after you see it snap.
03:56
Continue adding features to your single line.
03:60
From the Sketch toolbar, Create group, select the Center Diameter Circle command.
04:06
Hover to snap to the endpoint of the line, then Drag out and click to create a circle.
04:12
Similar to the line, you can adjust the circle diameter by clicking and dragging on the edge.
04:18
If you move the circle from its center point, notice that the line also moves with it,
04:23
since an automatic constraint was applied when you snapped to the endpoint.
04:27
Again, you can delete it by selecting the constraint and pressing Del or by using the Marking menu, if needed.
04:36
Before you can extrude to a 3D shape, your sketch must be a closed profile, meaning there are no gaps in the perimeter profile.
04:44
This is indicated by the light blue shading, as you can see with this circle.
04:49
To close an open profile, such as this box drawn around the circle, click on one vertex and snap it to another.
04:57
Now, you can start using some of these tools to create more complex sketches in Fusion.
05:03
For example, suppose you want to design a simple camera case, but first you need to design the camera itself as a reference model.
05:11
With a new design open, from the Browser, right-click the top-level node and select New Component.
05:18
In the New Component dialog, rename it something more appropriate, such as “Camera body”.
05:24
Make sure that Activate is selected, and click OK.
05:28
Then, click Create Sketch and select a plane to start a new sketch.
05:33
Before you start sketching, think about the simplest form you can achieve for your camera sketch.
05:38
In this case, a reference sketch, shows that the form is split up into two basic
05:44
bodies—the camera and the main body—that can form the base sketch for subsequent extrusion.
05:50
In Fusion, you can extrude multiple 3D features from just one sketch,
05:54
so both the main body and camera profiles can sit on one single 2D sketch profile.
06:00
With these shapes in mind, in the Sketch toolbar, Create group, click the Rectangle command
06:06
and create a two-point rectangle for the main body profile.
06:10
Click the canvas to place the start point, then click once more for the end point.
06:15
Once placed, notice the vertical and horizontal constraints have been automatically applied.
06:21
Now, using the Line command, create the camera sketch profile to approximately represent the camera by snapping to the lines.
06:30
Place it just above the automatic midpoint snapping, so you are not constrained to the midpoint of the line.
06:37
With your base sketch in position, you can now modify it by applying some fillets as 2D sketch features.
06:43
In the Modify group, select the Fillet command.
06:47
Select the connecting point between two lines in the sketch.
06:51
You can see a preview of the fillet in red, and after you click, you are prompted to enter the dimension.
06:57
Type a value, such as 10 and press Enter to apply the fillet and dimension.
07:03
To continue creating the other fillets, right-click to open the Marking menu, and select Repeat Fillet.
07:09
Select each of the other three corners, as well as the inner corner of the camera profile.
07:15
You stay in the fillet command and each of your selections has the same fillet radius as the first selected,
07:21
as an automatic equal constraint was applied.
07:29
Due to the equal constraint, you can see that all four selected fillets update to the same dimension.
07:36
The original fillet that you created is still set at 10 mm, as there is no relationship between this fillet and the other four.
07:44
Double-click the dimension for the original fillet and enter 5 mm.
07:49
You have two remaining fillets for the camera profile.
07:53
When you repeat the Fillet command for these two, notice that some of the automatically applied constraints are now lost.
08:00
Fusion cannot establish how to repair these as you have created a feature that has multiple points that it could connect to.
08:07
In this case, click the Line command again and repair these gaps, using automatic snapping.
08:14
Once finished, you can see the two closed profiles, as indicated by the light blue shading.
08:20
Your sketch might look a bit cluttered with all the constraints and dimensions on your screen.
08:25
From the Sketch Palette, deselect the Dimensions and Constraints checkboxes to hide these and make your workspace a little cleaner.
00:03
In Fusion, sketches are the underlying geometry that support the creation of 3D solid, surface, and T-Spline bodies in your design.
00:12
To access the sketch environment, in the Solid toolbar, Create group, click Create Sketch.
00:20
On the canvas, select the initial plane or face to begin the sketch on.
00:25
In this example, the XZ plane is selected, and the environment automatically aligns to this plane.
00:32
You can disable this in the Design Preferences by deselecting the Auto look at sketch checkbox.
00:38
Back in the sketch environment, notice that you now see the Sketch toolbar, indicated by the currently active Sketch tab.
00:46
From here, you have access to sketching features and tools that follow a typical sketching
00:52
workflow—first, you create your base outline shape, before modifying it, until finally constraining it.
00:59
The first section, the Create group, is where you can find basic shapes including lines, circles, and text to create your base sketch.
01:08
Other Create commands and tools include the Mirror and Pattern commands, the Project command, and the dimensioning tool.
01:16
Once you have a base sketch in place, you can use the tools in the Modify group, such as Fillet, Trim, or Offset.
01:24
Then, use the tools in the Constraints group to maintain complete control over your design and avoid unwanted errors.
01:32
The Sketch Palette also offers additional sketch tools to help with your workflow.
01:37
After this quick run through of the sketching UI, you are ready to create some basic shapes.
01:43
Start by creating a simple line.
01:46
In the Sketch toolbar, Create group, click the Line command.
01:51
You can also press the keyboard shortcut L for line, press S to search for a command,
01:57
or right-click the canvas to access the command from the Marking menu.
02:02
Once the command has been selected, you are prompted to place the first point.
02:07
You can place the first point anywhere on the canvas.
02:11
Here, use the origin as your starting point by hovering near to it, waiting for it to snap, then clicking to place.
02:18
Once placed, drag this line away from the origin.
02:22
You can see a preview of the line, as well as two dialog boxes that let you define the length and angle, if already known.
02:30
Also, if you drag this line to the X or Z axis, it snaps to the respective axis.
02:36
Both dialog boxes and automatic snapping provide quick ways to apply constraints and dimensions to your sketch.
02:44
Create a line that does not snap to the horizontal or vertical at any length and angle by clicking once you have your position.
02:51
After you place a second point, you can drag the line out to continue and create more lines.
02:57
Notice how you can also snap to other sketch features, such as a midpoint, or by creating a perpendicular line.
03:05
To leave this as a single line for now, click the green check mark to confirm.
03:10
You are still in the Create Line mode.
03:13
To end it, press Esc or Enter on your keyboard.
03:17
At the moment, this sketch is not fully defined, meaning you can move it around and change its length simply by dragging its end point.
03:25
As you snapped to and selected the origin for the starting position,
03:29
an automatic constraint was placed, meaning this start point is locked in place.
03:34
As such, you cannot move it as you have just done with the end point.
03:39
Click this start point to see the relative constraint symbol.
03:43
If you delete this to remove the constraint, the sketched line is now free to move.
03:49
To reset the constraint, simply drag the end point back to the origin and release the mouse button after you see it snap.
03:56
Continue adding features to your single line.
03:60
From the Sketch toolbar, Create group, select the Center Diameter Circle command.
04:06
Hover to snap to the endpoint of the line, then Drag out and click to create a circle.
04:12
Similar to the line, you can adjust the circle diameter by clicking and dragging on the edge.
04:18
If you move the circle from its center point, notice that the line also moves with it,
04:23
since an automatic constraint was applied when you snapped to the endpoint.
04:27
Again, you can delete it by selecting the constraint and pressing Del or by using the Marking menu, if needed.
04:36
Before you can extrude to a 3D shape, your sketch must be a closed profile, meaning there are no gaps in the perimeter profile.
04:44
This is indicated by the light blue shading, as you can see with this circle.
04:49
To close an open profile, such as this box drawn around the circle, click on one vertex and snap it to another.
04:57
Now, you can start using some of these tools to create more complex sketches in Fusion.
05:03
For example, suppose you want to design a simple camera case, but first you need to design the camera itself as a reference model.
05:11
With a new design open, from the Browser, right-click the top-level node and select New Component.
05:18
In the New Component dialog, rename it something more appropriate, such as “Camera body”.
05:24
Make sure that Activate is selected, and click OK.
05:28
Then, click Create Sketch and select a plane to start a new sketch.
05:33
Before you start sketching, think about the simplest form you can achieve for your camera sketch.
05:38
In this case, a reference sketch, shows that the form is split up into two basic
05:44
bodies—the camera and the main body—that can form the base sketch for subsequent extrusion.
05:50
In Fusion, you can extrude multiple 3D features from just one sketch,
05:54
so both the main body and camera profiles can sit on one single 2D sketch profile.
06:00
With these shapes in mind, in the Sketch toolbar, Create group, click the Rectangle command
06:06
and create a two-point rectangle for the main body profile.
06:10
Click the canvas to place the start point, then click once more for the end point.
06:15
Once placed, notice the vertical and horizontal constraints have been automatically applied.
06:21
Now, using the Line command, create the camera sketch profile to approximately represent the camera by snapping to the lines.
06:30
Place it just above the automatic midpoint snapping, so you are not constrained to the midpoint of the line.
06:37
With your base sketch in position, you can now modify it by applying some fillets as 2D sketch features.
06:43
In the Modify group, select the Fillet command.
06:47
Select the connecting point between two lines in the sketch.
06:51
You can see a preview of the fillet in red, and after you click, you are prompted to enter the dimension.
06:57
Type a value, such as 10 and press Enter to apply the fillet and dimension.
07:03
To continue creating the other fillets, right-click to open the Marking menu, and select Repeat Fillet.
07:09
Select each of the other three corners, as well as the inner corner of the camera profile.
07:15
You stay in the fillet command and each of your selections has the same fillet radius as the first selected,
07:21
as an automatic equal constraint was applied.
07:29
Due to the equal constraint, you can see that all four selected fillets update to the same dimension.
07:36
The original fillet that you created is still set at 10 mm, as there is no relationship between this fillet and the other four.
07:44
Double-click the dimension for the original fillet and enter 5 mm.
07:49
You have two remaining fillets for the camera profile.
07:53
When you repeat the Fillet command for these two, notice that some of the automatically applied constraints are now lost.
08:00
Fusion cannot establish how to repair these as you have created a feature that has multiple points that it could connect to.
08:07
In this case, click the Line command again and repair these gaps, using automatic snapping.
08:14
Once finished, you can see the two closed profiles, as indicated by the light blue shading.
08:20
Your sketch might look a bit cluttered with all the constraints and dimensions on your screen.
08:25
From the Sketch Palette, deselect the Dimensions and Constraints checkboxes to hide these and make your workspace a little cleaner.
