Use constraints and dimensions to fully define a sketch.
Transcript
00:03
With a basic sketch defined in Fusion, you can use the dimension tool and constrain features to turn your work into a fully defined sketch.
00:11
Here is an example to give you an idea of why you want to constrain your sketches.
00:16
These are two nearly identical sketches.
00:19
On the left is an unconstrained sketch, as indicated by the blue lines.
00:24
The sketch on the right is a fully defined sketch, as indicated by the black lines.
00:30
The difference is that the features of a fully defined sketch
00:33
have some dimensional or positional relationship with other sketch features.
00:38
This gives you more control over your design, while avoiding unwanted behaviors.
00:43
In the left sketch, you can move the points and edges in space.
00:48
While this gives you more freedom, it can lead to unpredictable and often unwanted behaviors.
00:55
If you attempt to move the same point and edge in the fully defined sketch, you are unable to do so.
01:02
In the right sketch, you have more control over your design,
01:06
as you can establish how features are updated depending on their relationship with other features.
01:11
In the Sketch Palette, if you select Show Dimensions and Show Constraints, you can see what is driving this.
01:18
For instance, if you edit one fillet, then the remaining three also update to the same value
01:24
because of the equal dimensions placed on them.
01:27
Similarly, the width updates with respect to the midpoint constraint placed on the sketch and the construction line,
01:33
and will not extend past this midpoint.
01:37
The aim here is to turn this unconstrained sketch on the left into a fully constrained sketch on the right
01:42
by using construction lines, constraints, and the dimension tool.
01:47
It is considered best practice to fully constrain your sketch before proceeding to 3D modeling.
01:53
Constraints place a positional or relational commonality between points or objects,
01:58
and depending on which constraint you select, you can limit the ability of the point or object to move freely in space.
02:05
In this camera case sketch, from the Sketch Palette, select Show Dimensions and Show Constraints.
02:11
You can see that there are already some automatically applied constraints,
02:15
including the tangent, vertical or horizontal, and equal constraints.
02:20
Although these can be placed automatically, to better understand constraints, delete and reapply these constraints manually.
02:28
Delete the tangent, equal, and horizontal constraint at the bottom of the sketch
02:32
by clicking each constraint and pressing Delete on your keyboard,
02:36
or by right-clicking and selecting Delete from the Markup menu.
02:40
Once these three constraints are deleted, you are free to move these particular sketch features in space.
02:46
First, replicate the horizontal constraint on the lower line.
02:51
Although it appears horizontal, it is always best to place a constraint.
02:55
On the Sketch contextual tab, Constraints group, click Horizontal/Vertical.
03:01
Select the line to lock it to a horizontal position.
03:05
This is confirmed by the horizontal constraint symbol next to it.
03:09
Now you want to create a tangent constraint between the lower line and the corner arc.
03:14
Select both sketch entities, right-click to open the Marking menu and select Tangent.
03:20
You can see that it has been applied by the tangent symbol next to the arc.
03:24
Next, you want to constrain the fillet so that it matches the other fillets.
03:29
However, instead of using the equal constraint, you can use the Dimension tool to reference another sketch dimension.
03:36
You can access the Dimension tool by pressing D, from the Marking menu, or from the Sketch tab, Create group.
03:43
With this tool, you can set linear or angular dimensions to any sketch feature.
03:49
To place a dimension, click on a feature or two features, then click again.
03:54
You then can enter a value of your choice before pressing Enter to confirm.
03:59
In the camera case example, open the Dimension tool and click on the undimensioned fillet.
04:04
As you want this fillet to be equal to another fillet, click on another fillet dimension, and then press Enter.
04:11
This dimension will now always equal the reference dimension of 5 mm.
04:16
If you update the reference value to 6 mm, the newly dimensioned fillet also updates.
04:22
The other fillet values do not update, as you have not applied an equal constraint or referenced the same dimension.
04:29
Repeat the dimensioning for the other fillets, then set the reference dimension back to 5 millimetres.
04:35
You can now create construction lines to define the upper and lower limits of your sketch.
04:41
A construction line is a useful tool for referencing your sketch and acting as a base when dimensioning other sketch features.
04:48
In this case, you want your construction lines to be exactly at the midpoints of the outer sketch profile,
04:54
so one method might be to use the automatically applied constraints, such as the midpoint.
04:59
Instead, a more in-depth method can help you understand the fundamentals of creating geometry and applying constraints manually.
05:07
On the Sketch tab, Create group, click the Line command.
05:11
Place the pointer over the origin point to snap to it, but do not click.
05:16
If you drag down, you can see the dotted line indicating that you are snapping to the Z axis.
05:22
This is an example of how you can use other sketch features to line up entities,
05:27
although you should note that no automatic constraints will be placed in this instance.
05:31
You want to create horizontal and vertical construction lines.
05:35
First, create a vertical line of a length that is approximately the same as the sketch.
05:41
Then repeat for the horizontal.
05:44
Go back to the origin to enable automatic snapping on this axis.
05:49
With these lines in place, note that there are now four separate profiles.
05:54
If you were to extrude this, you would need to select all four profiles.
05:59
By turning these into construction lines, they have no active involvement when you extrude, as you only have one profile.
06:06
Select the lines, and either press X, or from the Sketch Palette, click Construction.
06:12
The lines now appear as dotted construction lines and are free to move in space.
06:17
As these will be the basis of your sketch, you should constrain them,
06:21
so they are at midpoints with each other and their midpoints are then constrained to the origin.
06:26
Select both construction lines, right-click to open the Marking menu, and select MidPoint to place a constraint.
06:33
You are still in the midpoint mode, so select either line, then the origin, and both will snap to this point.
06:40
Now, you want to constrain the sketch, so the perimeter edges are always in line with the construction lines.
06:47
In this case, you can use a Coincident constraint, as you want to constrain the endpoint to the line.
06:52
On the Sketch tab, Constraints group, click Coincident.
06:57
Select the endpoint and its corresponding line to snap it into position.
07:01
Repeat for the other three endpoints and lines.
07:05
With these constraints in place, you are still not fully defined.
07:09
If you drag the lines, the construction lines move with it.
07:13
Also notice how the entities that represent the camera are not quite what you are expecting.
07:18
This is an example of issues that can occur if you do not fully define your sketch.
07:24
Drag the top line up for now so that it is easier to manage.
07:28
Place dimensions to establish what the vertical and horizontal dimensions are.
07:33
You can either select the upper and lower lines or the respective construction lines themselves, which are dependent on the constraints placed.
07:41
You can now finish off the camera portion of the sketch to make sure everything is fully defined.
07:46
As the sides are equal length, you can dimension one side, then use the equal constraint on the other.
07:53
Before you place the equal constraint, note the Sketch symbol in the Browser.
07:58
After you place the constraint, the symbol now has a lock indicating that it is a fully defined sketch,
08:03
and can only be edited by updating the dimension values.
08:07
You can also use equations in your dimensioning.
08:11
In this example, you want the camera to be exactly half of the main body.
08:16
First, click to edit the length dimension of the camera, then click on the main body length dimension as a reference, and finally, type “/2”.
08:25
After pressing Enter, you can now see the fx, indicating that it is referencing another dimension,
08:30
and it is also exactly half of the main body length.
08:34
If you update the main body length, the camera length also updates.
00:03
With a basic sketch defined in Fusion, you can use the dimension tool and constrain features to turn your work into a fully defined sketch.
00:11
Here is an example to give you an idea of why you want to constrain your sketches.
00:16
These are two nearly identical sketches.
00:19
On the left is an unconstrained sketch, as indicated by the blue lines.
00:24
The sketch on the right is a fully defined sketch, as indicated by the black lines.
00:30
The difference is that the features of a fully defined sketch
00:33
have some dimensional or positional relationship with other sketch features.
00:38
This gives you more control over your design, while avoiding unwanted behaviors.
00:43
In the left sketch, you can move the points and edges in space.
00:48
While this gives you more freedom, it can lead to unpredictable and often unwanted behaviors.
00:55
If you attempt to move the same point and edge in the fully defined sketch, you are unable to do so.
01:02
In the right sketch, you have more control over your design,
01:06
as you can establish how features are updated depending on their relationship with other features.
01:11
In the Sketch Palette, if you select Show Dimensions and Show Constraints, you can see what is driving this.
01:18
For instance, if you edit one fillet, then the remaining three also update to the same value
01:24
because of the equal dimensions placed on them.
01:27
Similarly, the width updates with respect to the midpoint constraint placed on the sketch and the construction line,
01:33
and will not extend past this midpoint.
01:37
The aim here is to turn this unconstrained sketch on the left into a fully constrained sketch on the right
01:42
by using construction lines, constraints, and the dimension tool.
01:47
It is considered best practice to fully constrain your sketch before proceeding to 3D modeling.
01:53
Constraints place a positional or relational commonality between points or objects,
01:58
and depending on which constraint you select, you can limit the ability of the point or object to move freely in space.
02:05
In this camera case sketch, from the Sketch Palette, select Show Dimensions and Show Constraints.
02:11
You can see that there are already some automatically applied constraints,
02:15
including the tangent, vertical or horizontal, and equal constraints.
02:20
Although these can be placed automatically, to better understand constraints, delete and reapply these constraints manually.
02:28
Delete the tangent, equal, and horizontal constraint at the bottom of the sketch
02:32
by clicking each constraint and pressing Delete on your keyboard,
02:36
or by right-clicking and selecting Delete from the Markup menu.
02:40
Once these three constraints are deleted, you are free to move these particular sketch features in space.
02:46
First, replicate the horizontal constraint on the lower line.
02:51
Although it appears horizontal, it is always best to place a constraint.
02:55
On the Sketch contextual tab, Constraints group, click Horizontal/Vertical.
03:01
Select the line to lock it to a horizontal position.
03:05
This is confirmed by the horizontal constraint symbol next to it.
03:09
Now you want to create a tangent constraint between the lower line and the corner arc.
03:14
Select both sketch entities, right-click to open the Marking menu and select Tangent.
03:20
You can see that it has been applied by the tangent symbol next to the arc.
03:24
Next, you want to constrain the fillet so that it matches the other fillets.
03:29
However, instead of using the equal constraint, you can use the Dimension tool to reference another sketch dimension.
03:36
You can access the Dimension tool by pressing D, from the Marking menu, or from the Sketch tab, Create group.
03:43
With this tool, you can set linear or angular dimensions to any sketch feature.
03:49
To place a dimension, click on a feature or two features, then click again.
03:54
You then can enter a value of your choice before pressing Enter to confirm.
03:59
In the camera case example, open the Dimension tool and click on the undimensioned fillet.
04:04
As you want this fillet to be equal to another fillet, click on another fillet dimension, and then press Enter.
04:11
This dimension will now always equal the reference dimension of 5 mm.
04:16
If you update the reference value to 6 mm, the newly dimensioned fillet also updates.
04:22
The other fillet values do not update, as you have not applied an equal constraint or referenced the same dimension.
04:29
Repeat the dimensioning for the other fillets, then set the reference dimension back to 5 millimetres.
04:35
You can now create construction lines to define the upper and lower limits of your sketch.
04:41
A construction line is a useful tool for referencing your sketch and acting as a base when dimensioning other sketch features.
04:48
In this case, you want your construction lines to be exactly at the midpoints of the outer sketch profile,
04:54
so one method might be to use the automatically applied constraints, such as the midpoint.
04:59
Instead, a more in-depth method can help you understand the fundamentals of creating geometry and applying constraints manually.
05:07
On the Sketch tab, Create group, click the Line command.
05:11
Place the pointer over the origin point to snap to it, but do not click.
05:16
If you drag down, you can see the dotted line indicating that you are snapping to the Z axis.
05:22
This is an example of how you can use other sketch features to line up entities,
05:27
although you should note that no automatic constraints will be placed in this instance.
05:31
You want to create horizontal and vertical construction lines.
05:35
First, create a vertical line of a length that is approximately the same as the sketch.
05:41
Then repeat for the horizontal.
05:44
Go back to the origin to enable automatic snapping on this axis.
05:49
With these lines in place, note that there are now four separate profiles.
05:54
If you were to extrude this, you would need to select all four profiles.
05:59
By turning these into construction lines, they have no active involvement when you extrude, as you only have one profile.
06:06
Select the lines, and either press X, or from the Sketch Palette, click Construction.
06:12
The lines now appear as dotted construction lines and are free to move in space.
06:17
As these will be the basis of your sketch, you should constrain them,
06:21
so they are at midpoints with each other and their midpoints are then constrained to the origin.
06:26
Select both construction lines, right-click to open the Marking menu, and select MidPoint to place a constraint.
06:33
You are still in the midpoint mode, so select either line, then the origin, and both will snap to this point.
06:40
Now, you want to constrain the sketch, so the perimeter edges are always in line with the construction lines.
06:47
In this case, you can use a Coincident constraint, as you want to constrain the endpoint to the line.
06:52
On the Sketch tab, Constraints group, click Coincident.
06:57
Select the endpoint and its corresponding line to snap it into position.
07:01
Repeat for the other three endpoints and lines.
07:05
With these constraints in place, you are still not fully defined.
07:09
If you drag the lines, the construction lines move with it.
07:13
Also notice how the entities that represent the camera are not quite what you are expecting.
07:18
This is an example of issues that can occur if you do not fully define your sketch.
07:24
Drag the top line up for now so that it is easier to manage.
07:28
Place dimensions to establish what the vertical and horizontal dimensions are.
07:33
You can either select the upper and lower lines or the respective construction lines themselves, which are dependent on the constraints placed.
07:41
You can now finish off the camera portion of the sketch to make sure everything is fully defined.
07:46
As the sides are equal length, you can dimension one side, then use the equal constraint on the other.
07:53
Before you place the equal constraint, note the Sketch symbol in the Browser.
07:58
After you place the constraint, the symbol now has a lock indicating that it is a fully defined sketch,
08:03
and can only be edited by updating the dimension values.
08:07
You can also use equations in your dimensioning.
08:11
In this example, you want the camera to be exactly half of the main body.
08:16
First, click to edit the length dimension of the camera, then click on the main body length dimension as a reference, and finally, type “/2”.
08:25
After pressing Enter, you can now see the fx, indicating that it is referencing another dimension,
08:30
and it is also exactly half of the main body length.
08:34
If you update the main body length, the camera length also updates.
