Project geometry onto a sketch plane

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In this video, you will learn how to use  the Project command to extract existing 2D  

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or 3D data to create referenced  geometry in your sketches.

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The project command is a tool that projects a body  silhouette or sketch geometries on to the active  

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sketch plane from existing geometry, and can only  be updated when the reference geometry is updated.

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This is useful when you want to create  equal geometry across separate sketches,  

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but only want to edit one sketch to  have the changes propagate across.

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In this example, you can see two components  in the assembly, and the four bolt holes on  

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the large end cap need to be projected  onto the sketch of the small end cap.

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The idea being that if you ever need to  change the bolt diameter or locations,  

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you won’t need to individually edit the values  for each hole on separate sketches or components,  

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thereby improving your workflow and  reducing the risk of downstream errors.

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Go ahead and edit the sketch  on our small end cap to begin.

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On the toolbar, in the Create menu, expand  the Project/Include menu, then select Project.

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Fusion 360 is asking to either  select individual geometry,  

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or an entire body. Individual geometry  includes lines, points, or arcs, for example,  

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whereas an entire body will project  a silhouette of the selected bodies.

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Leave this as specified entities for now,  

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then hover over the underlying holes on the  large end cap body until you see a red outline.  

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Fusion 360 is previewing the projected sketch,  and to select just left click on your mouse.

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You can continue adding geometry to the project  command, so repeat this for the other 3 holes.

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You will now see in the dialog that we have 4  items selected, and those items are shaded blue.

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If you ever add geometry by mistake you can always  left click on it to remove it from the selection.

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Make sure the ‘Projection Link’ is checked as  this confirms we want to create projected geometry  

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that will maintain an associative relationship  between the projected geometry and the active  

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sketch. If unchecked, then basic sketch  geometry without a reference will be created.

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Now press okay to confirm.

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Hide the dimensions and constraints  from the sketch palette,  

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as well as hiding the large end cap component.  

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You can now see the purple geometry on the small  end cap sketch which confirms it is projected.  

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If you click on one of the circles,  

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take note of its dimension in the  lower right hand corner of the canvas.

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To edit project geometry, you need  to edit the reference geometry.

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Go ahead and edit Sketch4 in the large end  cap to bring up the reference geometry.

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Here you can see the four holes,  with just one dimension placed  

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and the remainder with an equal constraint.

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You can double click on the dimension to edit it,  put in a value, press enter, then exit the sketch.

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Go back into the small end cap sketch and edit  it, and you will see the size of the holes have  

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updated even though the value was updated on  a separate sketch, on a separate component.

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One final feature is the ability to break these  projected links in the even you do not need  

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to maintain that associativity between  the projected sketch and its reference.

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To do this, right click on any projected  sketch geometry, then select Break Link.

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Now you have an unconstrained  sketch which you can edit to suit,  

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although note this operation cannot be reversed.

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Now you know how to project existing  geometry into a separate sketch  

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and reference it to drive a sketch profile  in a parametric design in Fusion 360.

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Thanks for watching.