Day 14 of Learn Fusion 360 in 30 Days for Complete Beginners! – 2026 EDITION – All 13 Autodesk Fusion Sketch Constraints Explained

Learn Autodesk Fusion in 30 Days (formerly called ‘Fusion 360’) is the most popular Fusion course online and was first launched in 2019. Since then, we have launched a revised 2023-24 version, and we are now releasing a fully updated and improved 2026 version.

This is Day #14 of the 2026 Revised version of the course.

Full Course on YouTube

Watch the full course in this official PDO YouTube playlist.

Sketch Constraints Challenge

1. Click the link to open the file: https://a360.co/4xekDfM
2. Click Open in Fusion (allow a minute for it to load).
3. Click Open when your browser asks for permission to launch the application.
4. Please note: You can delete the extra sketch and Extrude, which is only provided so Fusion’s shared link preview doesn’t say the ‘model is empty’ if the file contains only a sketch.
5. Then, download the challenge PDF (below)

Download the Sketch Constraint Challenge PDF

Get the 15-day Bundle of Companion Guide (Step-by-step PDFs)

Grab the official, step-by-step PDF guides and build your CAD mastery on a rock-solid foundation of practice projects and challenges. Serves as a standalone guide or the perfect companion to the video lessons.

Transcript

Change one single dimension, and your entire design twists into a chaotic mess. We’ve all been there, but that stops today. Welcome to Day 14 of Learn Fusion in 30 Days.

The biggest mistake Fusion beginners make is skipping sketch constraints to save time. The moment you need to make a simple edit later, you can lose hours fixing the broken geometry that cascades throughout your timeline.

Sketch Constraints help you define geometric relationships between lines and other sketch objects. They control the position of sketch objects and define exactly how your sketch geometry behaves. This makes your models stable, fast, and entirely predictable.

Today, you’ll sketch out a receptacle cover as you master all 13 sketch constraints, along with a fun challenge at the end to test your skills. Let’s dive in.

Start with a Part Design file and save your design. Press “L” to activate Line and start a new sketch on the bottom XY origin plane. In the Sketch environment, constraints live in the center of the toolbar, with the full list in the constraints menu.

Click twice to sketch a random line. Here’s a pro tip: whenever you place a line, double-click to end your continuous line segment while keeping the Line tool active. This saves you from pressing Escape and reactivating Line.

Let’s try it again. Click once to start the line, a second time for the second endpoint, then double-click as you place the second line, which terminates the continuous line.

Fusion always helps you and automatically applies sketch constraints as you sketch. If you see any visible sketch constraints, press the ESC key, and select them, and press Delete. You can also right-click the constraints and select Delete from the Marking menu.

The most used constraint in Fusion is the Coincident constraint.

Coincident allows you to ‘snap’ together two points or a point and a line. 

Activate Coincident from the toolbar and select the top two points. Notice: Coincident forces them to snap together. Let’s do it again. Select the bottom two endpoints to snap them together.

Let’s also click the bottom right point and force this to snap to our Origin point. Notice the constraints moved our entire sketch and glued it to the Origin.

Press ESC to clear the command, then click and drag the sketch geometry. The sketch stays locked to the Origin forever unless you delete that Coincident constraint.

Click and drag the corners around until you form a crooked rectangle shape.

To make the two sides of the rectangle match, activate the Parallel constraint. Click the two vertical lines. Parallel forces two lines to extend in the same direction, ensuring they never intersect.

If you press Escape and click and drag a corner, you’ll find the lines remain parallel at all times.

Let’s delete the parallel constraint.

Currently, the corner does not measure 90 degrees. You can force two objects to lie perpendicular—or 90 degrees to each other—using the Perpendicular constraint.

With Perpendicular active, select two adjacent lines and observe the 90-degree angle.

Apply this to only one corner, as we’ll now look at the second most common constraint. The Horizontal/Vertical constraint constrains a single line, or two points, to lie on either the horizontal or vertical axis, whichever sits closer to the current alignment.

Activate it and select the two nearly vertical lines. This forces them to snap perfectly vertical. If you select the bottom line, it forces it to become horizontal since it lies closer to the horizontal alignment.

Watch closely as I select the top line. You will see that Fusion throws an error message stating: “The sketch geometry is over-constrained.”

Over-constrained means you are trying to add a dimension or constraint that directly contradicts an existing one. Our Perpendicular constraint at the corner already forces the top line to remain horizontal.

Because Fusion cannot solve two conflicting mathematical equations at the same time, it blocks the action to prevent a broken sketch.

Let’s activate the Center Diameter Circle tool and sketch two different circles inside our rectangle, making them different sizes.

The Equal constraint forces two or more objects to remain identical in size. Activate Equal and select the two circles.

Press Escape and click and drag one of the circles. Notice they remain identical in size.

Select one circle and press Delete to remove it. When you delete sketch objects, Fusion removes all associated constraints.

If you want this circle to sit in the middle of the rectangle, you can leverage the Midpoint constraint. However, Midpoint requires a line to reference.

Activate the Line tool and let’s sketch a line from one corner to the opposite corner, carefully snapping to each corner.

Press Escape, right-click the line, and select Construction. Remember, construction lines help you position geometry without affecting the sketch profile and 3D modeling features.

Click the center of the circle and drag it to the middle of the construction line. Notice a triangle glyph appears, which indicates the exact midpoint of the line. Releasing your mouse as it snaps to the midpoint automatically applies the Midpoint constraint.

If you press Undo, you can always activate Midpoint and select the center of the circle and the line.

Let’s click and drag the rectangle to make it larger.

Activate the 2-Point Rectangle tool and let’s sketch two different rectangles to serve as the receptacle openings. One will sit above the circle and one below it.

Notice that Fusion automatically applied the horizontal and vertical constraints, saving you time from manually applying them.

Here’s another pro tip: If Fusion keeps forcing automatic constraints where you don’t want them, Hold CMD on Mac or CTRL on Windows to disable automatic snapping and sketch constraints. 

Activate the Line tool and sketch a line out in space.

Use the Midpoint constraint to force one endpoint to remain at the middle of the right vertical line, and the opposite endpoint to remain at the midpoint of the other vertical line.

Select the line, then press the keyboard shortcut letter “X” to turn this into a construction line.

In the constraint menu, you will find the Symmetry constraint. This allows you to constrain two or more objects so that they remain symmetrical. In other words, they stay identical to each other in relation to a common axis. Let’s use our newly created construction line as the axis of symmetry to force the two rectangles to remain symmetrical.

Activate Symmetry from the constraint menu. To apply the Symmetry constraint, first select the two objects you want to make symmetrical, then select the symmetry line.

For example, select the left line of the top rectangle, the corresponding line of the bottom rectangle, and then the symmetry line.

Repeat this for the remaining three sides of the rectangle. Very important, remember the horizontal line acts as a mirror line, so the bottom of the upper rectangle corresponds to the top of the lower rectangle.

Once you apply symmetry to all four sides, press Escape and click and drag any side to test it. The rectangles will now match at all times.

It’s important to note that you should use the Symmetry constraint with caution. It works completely fine on a simple sketch like this, but do not get carried away and use it heavily throughout your Fusion sketches, as it often causes sketch latency. In those cases, mirror or pattern the solid features instead.

We want to center the rectangle, and a few ways exist to accomplish this.

One option requires drawing a line connecting the top two lines at their midpoints, followed by applying a vertical constraint. This forces the rectangle to slide to the center.

Another option requires activating the Point tool and adding a single sketch point to the midpoint of any horizontal line of the rectangle.

This allows you to use the Horizontal/Vertical constraint to force it to stay on the same vertical line as the center point you created with the construction lines.

Many ways exist to achieve the same results with sketch constraints. Always focus on using the option that utilizes fewer constraints or construction geometry and keeps your sketches simpler.

Other than that, you should build your sketches based on your ‘Design Intent’—or the strategy of baking “intelligence” into your sketches and features so that when you edit a dimension later, the model scales, shifts, or updates exactly the way you intended.

Press Escape to clear any commands, hold down the Shift key, and select the four vertical lines of the inner rectangles. Press “X” to turn them into construction lines.

Activate the 3-Point Arc tool and select both ends of a rectangle. Watch carefully as I move the mouse position. Notice a Tangent glyph appears, indicating that an automatic Tangent constraint will apply here. The Tangent constraint forces an arc to remain tangent to connected geometry, resulting in smooth transitions. This matters most when you work on lofted shapes or other complex geometries.

In our case, you want to click to place the third point where it does not include the Tangent constraints. Then, repeat the 3-point arc for the remaining three ends.

Since these four arcs should always remain identical in size, activate Equal and select the top two arcs to force them to remain identical. Repeat this for the bottom two arcs.

You could then apply the Symmetry constraint to the top and bottom arcs, choosing the same construction line as the symmetry line. However, with Equal still active, we can add an additional Equal constraint to a top and bottom arc. This achieves the same result with fewer constraints.

Notice our sketch is starting to get filled with constraints and construction geometry.

Here’s a pro tip: despite the Sketch Palette being open all the time, a lot of beginners overlook the settings. It’s here that you can turn off the visibility of construction geometry, constraints, dimensions, and more. This helps immensely when you need to focus on a specific connection.

The next constraint is Concentric, which constrains two or more arcs, circles, or ellipses so they share the same center point.

Notice the center of each arc floats in space. Activate Concentric and select each arc. This forces the arc’s center to remain at that same point.

If you press Undo and Shift-click the two center points, you will see that the toolbar disables all constraints that cannot apply based on your selection. In our case, we could apply the Coincident constraint to achieve the same result.

As you continue to learn and use Fusion, you will often change your mind on how you want to constrain your sketch.

Perhaps we want the center of our rectangle to align with the Origin. Press ESC to clear any commands. Right-click on the right corner point and select ‘Delete Coincident’ to remove the constraint that we added earlier.

You can now click and drag the right line, and notice the whole sketch moves together because of the applied constraints.

Activate Coincident and apply it to the center and the Origin.

Our sketch is now centered to the Origin.

We’ll discuss the remaining 4 constraints. However, let’s first fully define our sketch by adding dimensions.

Activate the Sketch Dimension tool and select the center circle where the screw goes. This measures 4mm.

Define the radius of one of the arcs as 17mm. Our Equal constraint applies the value to all four.

Let’s define the overall height as 115mm and the overall width as 80mm.

Notice our sketch does not yet show as fully defined. We need two remaining dimensions for the outlet cutouts. Turn off the visibility of constraints in the Sketch Palette to make it easier to see. Add a height dimension to the cutout, setting this to 28mm.

Lastly, define the distance from the bottom of the cutout to the center as 6mm. This fully defines our sketch, and all of the sketch geometry turns from blue to black to confirm that status.

If you need to create a jumbo or ‘oversized’ cover, you can now update the overall height or width predictably, without breaking the sketch.

The Fix/Unfix constraint allows you to lock sketch geometry. The size and location of the sketch geometry lock completely, and the selected geometry turns green to indicate it is locked.

This instantly locks down complex, un-dimensioned shapes like imported DXF or SVG files. However, you can also use it on complex spline geometry, such as the splines from the Day 4 bottle.

Collinear is the next constraint. This one does not occur quite as commonly, but there may be a time when you need two or more objects to share a common line. They don’t have to touch or match the same length; they just have to point in the same direction along the same invisible track.

The Curvature constraint allows you to create smooth, G2 continuous curvature between a spline and another sketch curve. This advanced constraint often comes into play with surface modeling or lofting complex shapes.

Without getting into the details, the Tangent constraint creates G1 curves, while the Curvature constraint creates G2 curves.

Lastly, we have the new Polygon constraint that Autodesk released in March of 2026.

It allows you to constrain a closed profile that features the same length and equal angles, forcing it to remain a regular polygon. Because Fusion offers preset polygon sketch tools, you will use this one infrequently.

Time for your challenge! Grab the challenge sheet linked in the video description and follow the requirements to fully constrain the Fusion logo. 

I’ll see you on Day 15, where we’ll wrap up the first 15 days by creating a customizable painter’s pyramid!