• Fusion

Project geometry onto a sketch plane

Project existing 2D or 3D geometry onto a sketch plane and associatively reference the projected geometry in a sketch.


00:08

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

00:13

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

00:19

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

00:24

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

00:32

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

00:36

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

00:44

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

00:50

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

00:55

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

00:60

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

01:05

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

01:10

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

01:18

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

01:32

Fusion 360 is asking to either  select individual geometry,  

01:36

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

01:43

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

01:48

Leave this as specified entities for now,  

01:51

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

01:58

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

02:07

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

02:16

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

02:23

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

02:32

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

02:37

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

02:42

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

02:50

Now press okay to confirm.

02:52

Hide the dimensions and constraints  from the sketch palette,  

02:55

as well as hiding the large end cap component.  

03:02

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

03:08

If you click on one of the circles,  

03:11

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

03:21

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

03:26

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

03:34

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

03:37

and the remainder with an equal constraint.

03:39

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

03:51

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

03:56

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

04:09

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

04:14

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

04:19

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

04:27

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

04:30

although note this operation cannot be reversed.

04:36

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

04:40

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

04:45

Thanks for watching.

Video transcript

00:08

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

00:13

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

00:19

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

00:24

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

00:32

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

00:36

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

00:44

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

00:50

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

00:55

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

00:60

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

01:05

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

01:10

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

01:18

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

01:32

Fusion 360 is asking to either  select individual geometry,  

01:36

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

01:43

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

01:48

Leave this as specified entities for now,  

01:51

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

01:58

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

02:07

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

02:16

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

02:23

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

02:32

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

02:37

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

02:42

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

02:50

Now press okay to confirm.

02:52

Hide the dimensions and constraints  from the sketch palette,  

02:55

as well as hiding the large end cap component.  

03:02

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

03:08

If you click on one of the circles,  

03:11

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

03:21

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

03:26

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

03:34

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

03:37

and the remainder with an equal constraint.

03:39

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

03:51

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

03:56

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

04:09

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

04:14

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

04:19

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

04:27

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

04:30

although note this operation cannot be reversed.

04:36

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

04:40

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

04:45

Thanks for watching.

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