Learn how sketching is an essential part of any parametric CAD system.
Transcript
00:03
In Fusion, you can make your designs more manageable before turning them into 3D shapes.
00:09
With SolidWorks, when you first create a sketch, you can find the sketch features and tools for modifications in the toolbar,
00:16
and the same is the case with Fusion.
00:19
However, Fusion also includes constraints—known as relations in SolidWorks—in the toolbar,
00:25
giving you everything you need in one place.
00:27
You can easily customise your toolbar.
00:30
Click and drag a tool to move it, or even drag it off the toolbar to remove it.
00:36
Or, you can add a tool from the panel drop-down.
00:40
Select the three dots next to any command in the list and then click Pin to Toolbar.
00:45
Note that you can find the Pin to Shortcut selection here as well.
00:50
By pressing S on your keyboard, you can open the Shortcuts dialog box,
00:54
where your Pin to Shortcut selections are placed for commonly used commands.
00:59
There is also a search function here.
01:02
Start typing to find a command, and you can also quickly add it to the shortcuts.
01:07
When working with the sketch tools as in this example,
01:10
Fusion provides a pop-up Sketch Palette that provides additional options for the active sketch tool.
01:16
This helps improve your general workflow by providing instant access to actions like setting your construction lines,
01:23
changing the visibility of certain sketch details, and enabling 3D sketches.
01:29
To see how these work in Fusion, an example sketch is created and constrained.
01:34
First, a vertical construction line needs to be created.
01:38
The Line command is selected, with the intent to place it in the center of the valve body.
01:44
However, as you can see, it cannot snap to anything, as the valve body is a separate component.
01:51
In this case, the Project command is used on the top face of the valve body to establish the base of the bonnet.
01:58
This results in a sketch linked to the outside diameter of the valve body.
02:03
However, this is not needed, so the Break Link command is used to break the link.
02:08
Now, the vertical construction line can be placed from the toolbar or by pressing the shortcut L.
02:15
Then, the height is defined.
02:18
Now the new line can be converted into a construction line.
02:22
Select it and then press X, or click Construction in the Sketch Palette.
02:27
Next, a basic outline of the bonnet shape is drawn, with the intent to dimension and constrain later.
02:34
With Fusion, you do not have to switch between sketch features when creating your base design.
02:40
For example, if you create a line, then click and drag before releasing it, then Fusion starts to form an arc feature.
02:48
This allows you to create your sketches much more quickly.
02:52
Also, be aware that automatic constraints are placed when creating certain sketch features in a certain way, like SolidWorks.
02:60
In this sketch, you can see that perpendicular, parallel, and tangential constraints have been automatically applied,
03:08
as indicated by the glyphs.
03:10
If you do not want any of these constraints, you can simply delete the glyph to remove them.
03:16
A quick tip:
03:17
If you select two sketch features and then right-click, you will only see the constraints available for the selected sketch features.
03:25
This can both help keep you focused and save you modeling time.
03:29
Alternatively, using the toolbar, you can apply any number of constraints or sketch modifications,
03:36
including fillets, offsets, and dimensions—also known as smart dimensions in SolidWorks.
03:43
You can select either the command or the features first, then apply them until you have a fully constrained model.
03:50
Next, Fusion has a number of parameters that you can apply to your sketches.
03:55
In SolidWorks, you may be more accustomed to the terms global variables and linked dimensions.
04:02
These are similar in Fusion, but they are known as model parameters and user parameters.
04:08
Parameters are accessible from the Toolbar, Modify drop-down, Change Parameters option.
04:15
The Change parameters dialog lets you create parametric equations that drive key dimensions, quantities,
04:22
and other aspects of your Fusion design.
04:25
Model parameters are automatically created when you create timeline features or define dimensions,
04:31
and are separated based on the components and their underlying designs.
04:35
User parameters are custom parameters created by you,
04:39
and are particularly useful if you have a known set of specific constraints for the designed features, such as wall thicknesses.
04:47
Model parameters are for when you want to reference a pre-existing feature and need to establish or change the reference name.
04:54
These can then be applied to dimensions within your sketch.
04:58
You can also mark parameters here as favorites.
05:02
Click the star next to any parameter, and it will populate under the Favorites tab.
05:07
Now when you add or amend a dimension, you can type any character within that reference, and the list of favorite options will appear.
05:15
Note that you can also add simple or complex equations to your parameters,
05:20
and you can use existing dimensions simply by clicking them,
05:23
giving you even more control over your design.
05:26
Also, when you change the parameter value in the dialog box, you can see it propagate instantly across the design.
05:34
This allows you to review changes without needing to refresh the model.
00:03
In Fusion, you can make your designs more manageable before turning them into 3D shapes.
00:09
With SolidWorks, when you first create a sketch, you can find the sketch features and tools for modifications in the toolbar,
00:16
and the same is the case with Fusion.
00:19
However, Fusion also includes constraints—known as relations in SolidWorks—in the toolbar,
00:25
giving you everything you need in one place.
00:27
You can easily customise your toolbar.
00:30
Click and drag a tool to move it, or even drag it off the toolbar to remove it.
00:36
Or, you can add a tool from the panel drop-down.
00:40
Select the three dots next to any command in the list and then click Pin to Toolbar.
00:45
Note that you can find the Pin to Shortcut selection here as well.
00:50
By pressing S on your keyboard, you can open the Shortcuts dialog box,
00:54
where your Pin to Shortcut selections are placed for commonly used commands.
00:59
There is also a search function here.
01:02
Start typing to find a command, and you can also quickly add it to the shortcuts.
01:07
When working with the sketch tools as in this example,
01:10
Fusion provides a pop-up Sketch Palette that provides additional options for the active sketch tool.
01:16
This helps improve your general workflow by providing instant access to actions like setting your construction lines,
01:23
changing the visibility of certain sketch details, and enabling 3D sketches.
01:29
To see how these work in Fusion, an example sketch is created and constrained.
01:34
First, a vertical construction line needs to be created.
01:38
The Line command is selected, with the intent to place it in the center of the valve body.
01:44
However, as you can see, it cannot snap to anything, as the valve body is a separate component.
01:51
In this case, the Project command is used on the top face of the valve body to establish the base of the bonnet.
01:58
This results in a sketch linked to the outside diameter of the valve body.
02:03
However, this is not needed, so the Break Link command is used to break the link.
02:08
Now, the vertical construction line can be placed from the toolbar or by pressing the shortcut L.
02:15
Then, the height is defined.
02:18
Now the new line can be converted into a construction line.
02:22
Select it and then press X, or click Construction in the Sketch Palette.
02:27
Next, a basic outline of the bonnet shape is drawn, with the intent to dimension and constrain later.
02:34
With Fusion, you do not have to switch between sketch features when creating your base design.
02:40
For example, if you create a line, then click and drag before releasing it, then Fusion starts to form an arc feature.
02:48
This allows you to create your sketches much more quickly.
02:52
Also, be aware that automatic constraints are placed when creating certain sketch features in a certain way, like SolidWorks.
02:60
In this sketch, you can see that perpendicular, parallel, and tangential constraints have been automatically applied,
03:08
as indicated by the glyphs.
03:10
If you do not want any of these constraints, you can simply delete the glyph to remove them.
03:16
A quick tip:
03:17
If you select two sketch features and then right-click, you will only see the constraints available for the selected sketch features.
03:25
This can both help keep you focused and save you modeling time.
03:29
Alternatively, using the toolbar, you can apply any number of constraints or sketch modifications,
03:36
including fillets, offsets, and dimensions—also known as smart dimensions in SolidWorks.
03:43
You can select either the command or the features first, then apply them until you have a fully constrained model.
03:50
Next, Fusion has a number of parameters that you can apply to your sketches.
03:55
In SolidWorks, you may be more accustomed to the terms global variables and linked dimensions.
04:02
These are similar in Fusion, but they are known as model parameters and user parameters.
04:08
Parameters are accessible from the Toolbar, Modify drop-down, Change Parameters option.
04:15
The Change parameters dialog lets you create parametric equations that drive key dimensions, quantities,
04:22
and other aspects of your Fusion design.
04:25
Model parameters are automatically created when you create timeline features or define dimensions,
04:31
and are separated based on the components and their underlying designs.
04:35
User parameters are custom parameters created by you,
04:39
and are particularly useful if you have a known set of specific constraints for the designed features, such as wall thicknesses.
04:47
Model parameters are for when you want to reference a pre-existing feature and need to establish or change the reference name.
04:54
These can then be applied to dimensions within your sketch.
04:58
You can also mark parameters here as favorites.
05:02
Click the star next to any parameter, and it will populate under the Favorites tab.
05:07
Now when you add or amend a dimension, you can type any character within that reference, and the list of favorite options will appear.
05:15
Note that you can also add simple or complex equations to your parameters,
05:20
and you can use existing dimensions simply by clicking them,
05:23
giving you even more control over your design.
05:26
Also, when you change the parameter value in the dialog box, you can see it propagate instantly across the design.
05:34
This allows you to review changes without needing to refresh the model.
