Day 17 of Learn Fusion 360 in 30 Days for Complete Beginners! – 2023 EDITION – Learn all 12 Fusion 360 Sketch Constraints

Demo File

https://a360.co/3EBz5o5 (click the link > select ‘Open in Fusion 360’ > select Open, if prompted)

IMPORTANT NOTE: The demo file will say it’s empty because there are no 3D bodies. Don’t worry, the sketch is included in the file!

Transcript

Welcome to Day #17 of Learn Fusion 360 in 30 Days. I’m Kevin Kennedy,

and today we’ll look at manually applying each unique sketch constraint in Fusion 360.

In the previous lesson, we discussed why you should fully define your sketches with constraints and dimensions. Be sure to complete that first, if you haven’t already.

To get started, download the “constraints” demo file below and open it in Fusion 360. Please note that the file will say the model is empty since there are no 3D bodies. Rest assured, the sketch is actually included in the demo file.

We’ll start by opening the existing sketch by double-clicking on it in the parametric timeline. Remember that our Sketch environment places us in a contextual Sketch tab. That means this sketch tab will only appear while in the Sketch mode.

It’s here that you’ll find all 12 constraint types.

Constraints allow you to control the relative position of sketch geometry in Fusion 360. If you look at the constraint icons in the sketch menu you’ll see that sketch constraints use geometric expressions, with the exception of “Fix/Unfix.”

These sketch constraints will help us maintain predictable behaviors when we update our sketch’s dimensions. You’ll want to use sketch constraints to maintain the shape of your sketch so your sketch stays 100% predictable. Applying constraints and dimensions correctly will allow you to always know what will change within the given sketch.

Starting at the top of our constraints list, you’ll find the “Horizontal/Vertical” constraint. This constraint forces a line to snap horizontally or vertically, whichever orientation is the closest.

After activating the constraint, select the middle line. Notice it forces the line to stay vertical and the vertical glyph appears next to it.

The “horizontal/vertical” constraint is also commonly used to make points line up with one another. If I select the centerpoint of the circle and this endpoint of the line you’ll see that they are now forced to remain on the same horizontal line.

We can test this by pressing the Escape key to clear the command and clicking and dragging the sketch around. Be sure to select  “undo” after testing.

Let’s also add a Horizontal constraint to the top two lines of the sketch.

Second on the list is the “Coincident” constraint. Coincident forces the two selected sketch entities to touch.

To add a Coincident Constraint we can select a point,  line, or curve to join them together. Let’s select this line first. You’ll then find that Fusion 360 will only allow us to select certain geometry, such as sketch points. 

I’ll select the end point of our vertical line. Notice this forces the line to move up to the horizontal line, forcing them to remain touching.

At any time, press the Escape key to clear the active Sketch Constraint. We can then click and drag on the horizontal line. Notice this vertical line will always stay connected because of the coincident constraint.

Select where two objects meet to see what constraint is keeping them together. You can always select the glyph and look for the name of the constraint in the lower right corner.

The third constraint on our list is the “Tangent” constraint, which constrains a curve and another object so that they touch at a single point but never cross each other. The tangent constraint will help us create a smooth transition between a line and a curve.

Let’s add the Tangent constraint to the arc and the nearby lines by first selecting the arc, followed by the right line. We’ll complete this for the left side by selecting the arc again, followed by the left line.

You’ll see that both lines are now tangent to the arc.

Fourth on our list is the “Equal” constraint. This constraint forces two entities to remain equal in size. A common beginner mistake I see is when users apply the same sketch dimension to many sketch entities. Avoid doing so, by first applying the Equal constraint. That allows us to only dimension one of the equal lines.

Once active, let’s select the two horizontal lines at the top. Notice it forces them to remain equal in size. We can test this by dragging one of the endpoints around and you’ll find they stay equal in size.

The next constraint is the “Parallel” constraint, which makes any two lines parallel to each other. Select the parallel constraint to activate it and then select these two lines.

We can now drag them around and they will always stay parallel to one another.

Generally, you’ll use the Parallel constraint when a line is not in the horizontal or vertical direction.

The next constraint is the “Perpendicular” constraint. This constraint forces two lines to remain at a 90-degree angle to one another.

An important thing to note is that the Perpendicular constraint does not have to be used on lines that are touching. Select the leftmost line, followed by the top horizontal line. You’ll see this makes them Perpendicular to one another.

Let’s also add perpendicular constraints to these two corners, making sure they remain a perfect 90 degrees.

Next, you’ll see the “Fix/Unfix” constraint. This command is unique in that it locks the size and location of a point or object.

Fix/Unfix should be used sparingly. It works best on Spline geometry or other objects, such as Exploded Text, that are hard to fully constrain. Otherwise, the Fix constraint will prevent your sketch from adapting to changes in dimensions or other constraints.

When applied, the “Fix” constraint will make the geometry green to indicate that it’s fixed. 

Next is the “Midpoint” constraint, which is represented by a triangle. This constraint will be used frequently when sketching in Fusion 360 and helps us force the endpoint of a line to the center point of another line or arc.

Let’s select the endpoint of this middle line and then select the bottom horizontal line. You’ll see it snaps to the midpoint and the triangle glyph now appears.

Let’s repeat this to the top of the line, making sure we select the endpoint of the vertical line and not the line itself. We’ll then select the line above.

Perhaps, we also want to add a Perpendicular constraint between these two lines to make sure they remain connected at a perfect 90 degrees.

The “Concentric” constraint helps us force circular sketch elements, such as circles and arcs, to share a common center point. 

For example, if we want this circle to share the same center point as the Arc, we can select both the Circle and the Arc. Notice both entities now share the same center point, which is represented by the concentric glyph.

Next on the list is the “Collinear” constraint, which forces two lines to share a single axis. They can be at any angle and do not have to be vertical or horizontal lines. The order in which you select the lines does matter if the lines are not horizontal or vertical.

Let’s simply apply this to the top two horizontal lines. This will force the two lines to share the same line.

Next up is the Symmetry Constraint. This constrains two or more objects so they are symmetrical throughout the sketch.

Let’s select the two outside lines. We’re then required to select our symmetry line. Let’s use our vertical line.

Notice they now have the symmetry glyph. If we move either one, the other one will remain the same distance from the center line.

As we move this geometry, you’ll find all of our previously applied sketch constraints are working together to keep the geometry intact. 

Last but not least, we have the “Curvature” constraint. This one is used less frequently but will come in handy when working on complex curvature. 

The “Curvature” constraint constrains two or more objects to create a smooth continuous curvature between them.

To demo this constraint, I’ll draw some sketch geometry on the side, starting with a straight line.

I’ll then draw a Fit Point Spline that starts from the top of the line.

Currently, this geometry does not include a smooth transition between the line and the spline. We can better visualize this by selecting the spline and turning on the ‘Curvature Comb’ in the Sketch Palette. This helps us see the curvature of a Spline or curve.

Activate the Curvature constraint and select the Spline and straight line. Notice this adjusts our Spline to create a smooth, continuous curve with G2 continuity. We won’t discuss what that means as it’s an advanced concept, but note that this continuity is ideal for achieving smooth geometry.

Notice the red line now transitions into the line, where before there was a stark cutoff. 

Let’s wrap up with a few helpful tips.

Right-clicking on any sketch entity will show you all of the relevant sketch constraints. 

You can select multiple sketch objects while holding the Shift key, followed by selecting the constraint. Many find this to be more efficient.

When sketching geometry, you can hold the Command key on your Mac or the Control key on Windows to stop the automatic Sketch constraints.

[Upbeat Music]

I’ll see you on Day #18 where we’ll look at converting STL files into editable files.

[End Upbeat Music]