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