Design a Planetary Gear Toy in Onshape

Model a 3D-printable planetary gear fidget toy using parametric CAD.

Introduction

30 Second Summary

Fidget toys are satisfying to spin, but one you designed yourself from scratch is on another level. Even better when you designed it collaboratively with someone else in real time.

In this project, you will design a planetary gear fidget toy with your dad in Onshape, then 3D print it at your library makerspace. You'll learn parametric modeling, custom FeatureScripts, Boolean operations, and assembly animations along the way.

What You'll Build

A planetary gear fidget toy where three small planet gears orbit inside a ring gear when you spin the central sun gear, demonstrating mechanical gear reduction with a 4:1 ratio.

By the end of this project, you'll have:

A fully modeled planetary gear set (sun gear, 3 planet gears, ring gear, and housing) designed collaboratively in a shared Onshape document.
A working assembly with revolute mates and gear relations that animates correctly, proving your gears mesh.
Exported STL files ready to 3D print a functional fidget toy at your library makerspace.
Secret Mission: Convert to herringbone (double-helix) teeth so the entire mechanism prints as one piece with no assembly required.

Are there any prerequisites?

Both you and your collaborator need existing Onshape Free accounts and basic Onshape experience (sketching, extruding, and navigating the interface). You'll also need access to a 3D printer at your library makerspace for the final print.

Before We Start

Before We Start...

Set Up the Shared Document and Add the Spur Gear FeatureScript

A planetary gear set has multiple interlocking parts that must mesh with mathematical precision. If one gear's tooth count or module is off by even a fraction, the whole mechanism jams.

Working in a shared Onshape document lets you and your collaborator model different components simultaneously. In this step, you'll create that shared workspace, add the custom gear-generation tool, and define the parameters that keep every gear consistent.

In this step, get ready to:

Create a shared Onshape document with edit access for both collaborators.
Add the Spur Gear FeatureScript to the document's Feature toolbar.
Define shared variables (module, teeth counts, depth, backlash) in a Variable Studio.

Create and share the Onshape document

One person will create the document and invite the other. Once both are inside, you'll see each other's colored cursors moving in real time.

In your browser, go to cad.onshape.com and sign in with your Onshape Free account.
Click the blue Create button in the top left corner.
Select Document... from the dropdown.
Name the document Planetary Gear Fidget and click OK.
Click the Share button in the top right corner of the document.
Enter your collaborator's email address in the sharing field.
Set the permission to Can edit and click Share.
Ask your collaborator to open the document from their Onshape account (it will appear in their Shared with me section).

Once both of you have the document open, you should see each other's colored cursors in the graphics area.

What is real-time collaboration in Onshape?

Onshape works like Google Docs for CAD. Both collaborators edit the same document simultaneously with no file conflicts or version confusion. Each person gets a colored cursor so you can see where the other is working.

For best performance, Onshape recommends 4 or fewer simultaneous editors per document.

Don't see your collaborator's cursor?

Make sure the other person opened the shared document (not a different personal document). Both users must be in the same workspace tab at the same time for cursors to appear.

If the document doesn't appear in your collaborator's account, check that you entered the correct email address in the Share dialog.

Help me troubleshoot why I can't see my collaborator in Onshape.

Add the Spur Gear FeatureScript to the toolbar

The Spur Gear FeatureScript is a community-built custom feature that generates mathematically correct involute gear profiles. Adding it to your toolbar gives you a one-click gear generator instead of sketching complex tooth curves manually.

In your document, make sure you are on the Part Studio 1 tab at the bottom of the screen.
Look at the Feature toolbar at the top. Click the + button at the right end of the toolbar (this opens the custom features dialog).
In the search box at the top of the dialog, paste this URL:

https://cad.onshape.com/documents/5742c8cde4b06c68b362d748/w/b493e0cb681bbf9497d9f4b3/e/c72760543a0d4412e72f6d38

The dialog will display the Spur Gear feature by Neil Cooke. Click the Spur Gear icon to add it to your toolbar.
Close the dialog. You should now see the Spur Gear icon in your Feature toolbar.

Why paste a URL instead of searching by name?

Onshape's custom features dialog lets you search by document name or paste a direct URL. Pasting the URL takes you straight to the correct document, avoiding confusion with similarly-named features from other authors.

Adding a custom feature to your toolbar is an account-level setting. The icon will appear in all of your documents, not just this one. Your collaborator sees it instantly because you're both in the same workspace.

Don't see the Spur Gear icon in the toolbar?

Make sure you clicked the gear icon itself in the dialog (not just the document name). The feature only appears on your toolbar after you select it.

If the URL doesn't load a result, try searching for Spur Gear in the search box and look for the one authored by Neil Cooke.

Help me add the Spur Gear FeatureScript to my Onshape toolbar.

Create the Variable Studio with shared parameters

A Variable Studio holds named values that every Part Studio and Assembly in your document can reference. By defining gear parameters here once, any change (like adjusting the module) automatically updates every gear that references it.

Click the + icon (Insert new tab) at the bottom left of the screen, next to the existing tabs.
Select Create Variable Studio.
A new tab opens with an empty variable table. Enter the following 6 variables, pressing Tab to move between fields after each entry:

Name: Module / Type: Length / Value: 1.5 mm.
Name: SunTeeth / Type: Number / Value: 15.
Name: PlanetTeeth / Type: Number / Value: 15.
Name: RingTeeth / Type: Number / Value: 45.
Name: GearDepth / Type: Length / Value: 10 mm.
Name: Backlash / Type: Length / Value: 0.1 mm.

Check the box at the bottom of the Variable Studio tab that says Insert into all Part Studios and Assemblies. This makes the variables accessible everywhere in the document.
Right-click the Variable Studio tab at the bottom and rename it to Variables so it's easy to find later.

What do these parameters control?

Module sets the tooth size (1.5 mm is large enough for FDM 3D printers to reproduce cleanly). SunTeeth, PlanetTeeth, and RingTeeth define how many teeth each gear has. The formula Ring = Sun + 2 x Planet (45 = 15 + 2 x 15) ensures the gears mesh correctly.

GearDepth is how thick each gear is. Backlash adds a tiny 0.1 mm gap between teeth to compensate for 3D printing tolerances where parts tend to come out slightly larger than modeled.

Why use a Variable Studio instead of typing values directly?

This is parametric modeling in action. If you later decide to change the module to 2 mm for larger teeth, you update it in one place and every gear regenerates automatically. Without variables, you'd manually edit each gear feature individually.

Confirm that both collaborators can see the Variable Studio tab with all 6 parameters defined. Your collaborator should also see the Spur Gear icon in the Feature toolbar.

Variables not showing up for your collaborator?

Make sure you checked the Insert into all Part Studios and Assemblies checkbox at the bottom of the Variable Studio tab. Without this, the variables stay local to the Variable Studio and won't be available in Part Studios.

Variable names must use only alphanumeric characters and underscores. If you see an error, check for spaces or special characters in the name field.

Help me fix my Variable Studio setup in Onshape.

Your shared workspace is ready with all the tools and parameters you need. Next up, you and your collaborator will split up to model the gears in parallel. One person builds the sun and planet gears while the other builds the ring gear and housing.

Model the Sun Gear and Planet Gears

Your shared document is set up, your variables are defined, and the Spur Gear FeatureScript is ready in the toolbar. Now it is time to model the actual gears that form the heart of your planetary mechanism.

This step is for Person A. While you build the sun gear and planet gears here, Person B can work on the ring gear and housing simultaneously in a separate Part Studio. This is the collaboration payoff of working in Onshape. Two people model different components at the same time, in the same document, without conflicts.

In this step, get ready to:

Create a sun gear at the origin using the Spur Gear FeatureScript.
Create a single planet gear at the correct center distance from the sun.
Pattern the planet gear into 3 copies spaced evenly around the sun.

Create the sun gear at the origin

The sun gear sits at the center of the planetary mechanism. Every other gear revolves around it, so it needs to be placed precisely at the origin.

Click the Insert new tab icon (the + button) at the bottom left of your Onshape interface.
Select Create Part Studio from the menu.
Right-click the new tab at the bottom and select Rename. Name it Sun and Planets.
Click the Sketch tool in the Feature toolbar.
Select the Top plane as your sketch plane.
Place a single point at the origin (the center crosshair). This point tells the Spur Gear FeatureScript where to generate the gear.
Click the green checkmark to accept and close the sketch.

Now invoke the Spur Gear feature to generate the sun gear.

Click the Spur Gear icon in the Feature toolbar (the custom feature you added in Step 1).
Set Module to 1.5.
Set Number of Teeth to 15.
Set Gear Depth to 10 mm.
Set Profile Offset (backlash) to 0.1 mm.
Set Center Bore to 5 mm.
Click the green checkmark to generate the gear.

A 15-tooth sun gear should now appear at the origin in your Part Studio. You can orbit the view (middle mouse button) to see the 3D tooth profile.

What do these parameters mean?

Module controls how large each tooth is. A module of 1.5 keeps teeth large enough to print cleanly on a standard FDM 3D printer with a 0.4 mm nozzle.

Profile Offset adds a tiny gap (backlash) between meshing teeth. Without it, 3D-printed gears would jam because FDM parts tend to come out slightly larger than modeled.

Center Bore creates a hole through the gear center for a shaft or axle pin.

Don't see the Spur Gear icon?

Make sure you are inside the Sun and Planets Part Studio tab, not the Assembly or Variable Studio. Custom features only appear in Part Studio tabs.

If the icon still does not appear, return to Step 1 and re-add the Spur Gear FeatureScript from the custom features menu.

Help me troubleshoot my missing Spur Gear feature.

Create one planet gear at the correct center distance

Planet gears mesh with both the sun gear and the ring gear. Their center distance from the sun is determined by a formula based on tooth counts and module.

How is the planet center distance calculated?

The formula is: (Sun teeth + Planet teeth) / 2 x Module. With your values: (15 + 15) / 2 x 1.5 = 22.5 mm. This places each planet gear exactly where its teeth mesh with the sun.

In the same Sun and Planets Part Studio, click the Sketch tool again.
Select the Top plane as the sketch plane.
Place a point at 22.5 mm from the origin along the X-axis. You can click to place the point, then add a dimension constraint of 22.5 mm from the origin.
Click the green checkmark to accept and close the sketch.
Click the Spur Gear icon in the Feature toolbar.
Set Module to 1.5.
Set Number of Teeth to 15.
Set Gear Depth to 10 mm.
Set Profile Offset to 0.1 mm.
Set Center Bore to 3 mm.
Click the green checkmark to generate the planet gear.

You should now see two gears in your Part Studio. The smaller bore planet gear sits 22.5 mm to the right of the sun gear. Check the parts list on the left side of the screen to confirm you have 2 separate parts listed.

Why is the planet bore smaller?

The sun gear has a 5 mm bore because it connects to a larger central shaft. The planet gears only need a 3 mm bore for thin pins that let them spin freely in the housing.

Planet gear overlapping the sun gear?

Double-check that your sketch point is exactly 22.5 mm from the origin, not from the edge of the sun gear. If the dimension constraint references the wrong geometry, the gears will overlap.

My planet gear is overlapping the sun gear. How do I fix the sketch point distance?

Pattern the planet gear into 3 evenly spaced copies

A planetary gear set needs multiple planet gears to distribute the load evenly. You will use Onshape's Circular Pattern feature to create 3 planets spaced 120 degrees apart around the sun.

Click Circular Pattern in the Feature toolbar (under the pattern tools dropdown).
Set Pattern type to Part.
In the Entities to pattern field, select the planet gear body (click on it in the viewport or the parts list).
Click in the Axis of pattern field. Select the Y-axis line through the origin (you can pick it from the origin triad or click the top face edge of the sun gear bore).
Set Instance count to 3. This includes the original seed, so Onshape creates 2 additional copies for a total of 3 planet gears.
Check Equal spacing and set the Angle to 360 degrees. This distributes the 3 planets evenly (120 degrees apart).
Click the green checkmark to confirm the pattern.

Your parts list should now show 4 parts total: 1 sun gear and 3 planet gears arranged symmetrically around it.

Why 3 planet gears?

Three planets provide balanced load distribution. The tooth count formula also requires that (Sun teeth + Ring teeth) / Number of planets is a whole number. With 15 + 45 = 60 and 60 / 3 = 20, the math checks out.

Only seeing 2 parts in the list?

Make sure you selected the planet gear part as the entity to pattern, not the Spur Gear feature. A Part pattern creates new separate parts. A Feature pattern would add material to the same body.

Also confirm that Instance count is set to 3, not 2. The instance count includes the original seed gear.

My Circular Pattern is not creating 3 separate planet gear parts. What am I doing wrong?

Your sun gear and 3 planet gears are complete. While you were building these, Person B has been modeling the ring gear and housing in their own Part Studio. In the next step, you will come together to assemble all the pieces and watch them animate.

Model the Ring Gear and Housing

While Person A builds the sun gear and planets, Person B tackles the outer structure that holds everything together. The ring gear is the stationary outer gear with internal teeth that mesh with the planet gears.

In this step, you will create an internal ring gear using a clever technique. You will generate a normal external gear, then subtract it from a solid cylinder to leave internal teeth behind. You will also model the housing caps that hold the assembly together.

In this step, get ready to:

Generate a 45-tooth external spur gear as a Boolean cutting tool.
Create the ring gear body using Boolean subtraction.
Model top and bottom caps with center and pin holes.

Create the 45-tooth external spur gear

The Spur Gear FeatureScript only generates external gears. To create internal teeth, you first generate a standard external gear, then use it as a cutting tool in a Boolean subtraction.

Click the + icon (Insert new element) in the bottom-left of the tab bar.
Select Create Part Studio from the menu.
Right-click the new tab at the bottom and rename it to Ring and Housing.
In the new Part Studio, click the Sketch tool in the Feature toolbar.
Select the Top plane as the sketch plane.
Place a single point at the origin using the Point tool.
Click the green checkmark to accept the sketch.
Click the Spur Gear icon in the Feature toolbar.
Set Module to 1.5.
Set Number of Teeth to 45.
Set Gear Depth to 10 mm.
Set Profile Offset (backlash) to 0.1 mm.
Click the green checkmark to generate the gear.

A large 45-tooth external spur gear appears at the origin. You will not keep this gear as a final part. It serves only as a cutting tool in the next substep.

Why generate an external gear if you need internal teeth?

The Spur Gear FeatureScript does not directly generate internal (ring) gears. The standard approach is to generate a normal external gear, then subtract its body from a larger cylinder. The void left behind has the exact involute tooth profile you need on the inside wall.

Don't see the Spur Gear icon in the toolbar?

The FeatureScript was added in Step 1. If it is missing, click the + button at the end of the Feature toolbar, select Add custom features, and search for "Spur Gear" by Neil Cooke.

help me add the Spur Gear FeatureScript to my toolbar

Create the ring gear body with Boolean subtraction

Now you will create a solid cylinder that is slightly larger than the external gear, then subtract the gear body from it. The result is a ring with internal teeth.

Start a new sketch on the Top plane.
Draw a circle centered at the origin with a diameter of 76 mm.
Click the green checkmark to accept the sketch.
Click the Extrude tool in the Feature toolbar.
Select the circle region you just sketched.
Set the Result type to New.
Set the depth to 12 mm. This is 1 mm extra on each side of the 10 mm gears to form a lip.
Click the green checkmark to create the cylinder.

You now have two parts in the Part Studio: the 45-tooth external gear and the 76 mm cylinder. Time to subtract.

Click the Boolean tool in the Feature toolbar.
Set the operation type to Subtract.
Click in the Tools field and select the 45-tooth gear body in the graphics area. This is the shape you are removing.
Click in the Targets field and select the cylinder. This is the part being cut.
Leave Keep tools unchecked so the external gear body is deleted after subtraction.
Click the green checkmark to accept the Boolean.

The cylinder now has 45 internal gear teeth cut into it. If the original external gear body still appears in the parts list, right-click it and select Delete.

What does the Boolean subtract do here?

Boolean subtract removes one solid body from another. The external gear acts as a cookie cutter. Where its teeth were, there is now empty space inside the cylinder. The remaining material forms the internal tooth profile that the planet gears will mesh with.

Boolean showing an error?

The gear and cylinder must physically overlap for Boolean to work. Make sure the cylinder diameter (76 mm) is larger than the gear's outer diameter, and that both parts are centered at the origin on the same plane.

Also verify that you selected the gear as the Tool and the cylinder as the Target. Swapping them would hollow out the gear instead of the cylinder.

help me fix the Boolean subtract error in my ring gear Part Studio

Model the top and bottom caps

The housing caps close off the top and bottom of the ring gear. They include holes for the sun gear shaft and planet gear pins to poke through.

Start a new sketch on the top face of the ring gear body.
Draw a circle centered at the origin with a diameter of 76 mm.
Click the green checkmark to accept the sketch.
Click Extrude and select the circle region.
Set the Result type to New (this creates a separate part from the ring body).
Set the depth to 1.5 mm upward (away from the ring body).
Click the green checkmark to create the top cap.

Now add the shaft and pin holes to the top cap.

Start a new sketch on the outer face of the top cap.
Draw a circle at the origin with a diameter of 5 mm. This is the center hole for the sun gear shaft.
Draw a circle at 22.5 mm from the origin (along the X-axis) with a diameter of 3 mm. This is the first planet gear pin hole.
Click the green checkmark to accept the sketch.
Use Circular Pattern on the 3 mm hole sketch: set the axis to the Y-axis through the origin, count to 3, with equal spacing (120 degrees apart).
Click Extrude and select all four hole regions (one center hole and three pin holes).
Set the Result type to Remove and set the End type to Through all.
Make sure the Merge scope targets the top cap part.
Click the green checkmark. The top cap now has a 5 mm center hole and three 3 mm pin holes.

Finally, create the bottom cap as a separate part so the gears can be inserted during assembly.

Start a new sketch on the bottom face of the ring gear body.
Draw a circle centered at the origin with a diameter of 76 mm.
Click the green checkmark to accept the sketch.
Click Extrude and select the circle region.
Set the Result type to New.
Set the depth to 1.5 mm downward (away from the ring body, opposite direction from the top cap).
Click the green checkmark to create the bottom cap.
Repeat the same hole pattern on the bottom cap: sketch a 5 mm center circle and a 3 mm circle at 22.5 mm from origin, use Circular Pattern for 3 pin holes, then Extrude with Remove and Through all targeting the bottom cap.

Why is the bottom cap a separate part?

If both caps were permanently fused to the ring, you would have no way to insert the gears during physical assembly. The bottom cap remains a separate part so you can drop in the sun and planet gears, then press-fit or glue the cap on afterwards.

Check the Parts list in the bottom-left panel of your Part Studio. You should see 2-3 parts listed: the ring gear body, the top cap, and the bottom cap.

Parts list showing extra parts?

If you still see the original 45-tooth external gear body, it was not removed during the Boolean subtract. Right-click it in the Parts list and select Delete. Only the ring body and caps should remain.

help me clean up extra parts in my Onshape Part Studio after Boolean subtraction

Your ring gear and housing are complete. In the next step, you and your collaborator will bring all the parts together in an assembly, add mates and gear relations, and animate the entire mechanism to verify the teeth mesh correctly.

Assemble, Animate, and Verify the Gear Set

Both Part Studios are complete. Person A built the sun gear and three planet gears. Person B built the ring gear and housing caps.

Now you will bring all of these parts together into a single Assembly to prove they mesh and spin correctly before sending anything to the 3D printer.

In this step, get ready to:

Insert all gear parts and set up Revolute mates so each gear can spin independently.
Add Gear Relations that lock the rotation ratios between sun, planet, and ring gears.
Animate the assembly and verify teeth mesh without collision using Follow Mode.

Insert parts and create Revolute mates

An assembly in Onshape defines how parts move relative to each other. You fix one part in place, then add mates that describe the allowed motion for everything else.

In the shared Planetary Gear Fidget document, click the + icon (Insert new tab) at the bottom of the screen.
Select Create Assembly.
Right-click the new Assembly tab and rename it Planetary Assembly.

You now have an empty assembly workspace ready for parts.

Click Insert in the Assembly toolbar (top left).
In the Insert dialog, navigate to the Ring and Housing Part Studio tab.
Select the ring gear body and click in the graphics area to place it.
Close the Insert dialog.
Right-click the ring gear in the graphics area or the feature list on the left, then select Fix.

Why fix the ring gear?

In a planetary gear system, the ring gear stays stationary while the sun and planets move. Fixing it removes all six degrees of freedom so every other part mates relative to it.

Click Insert again and navigate to the Sun and Planets Part Studio tab.
Select the sun gear and place it in the graphics area.
Close the Insert dialog.
Click Revolute Mate in the Assembly toolbar.
For the first mate connector, hover over the center bore hole on the sun gear and select the center point on the top face.
For the second mate connector, select the center point of the ring gear's center hole.
Click the green checkmark to accept the mate.

What is a Revolute mate?

A Revolute mate allows rotation around a single axis (the Z-axis of the mate connector). The sun gear can now spin freely at the center of the ring gear without sliding sideways.

Next, insert and mate all three planet gears.

Click Insert and navigate to the Sun and Planets Part Studio.
Select all 3 planet gears and place them in the graphics area.
Close the Insert dialog.
For the first planet gear, click Revolute Mate in the toolbar.
Select the center bore top-face point on the planet gear as the first connector.
For the second connector, select a point on the ring gear at 22.5 mm from center along the X-axis (0 degrees). Use Flip Primary Axis or Rotate Secondary Axes if the gear orientation looks wrong.
Accept the mate with the green checkmark.
Repeat the Revolute mate process for the second planet gear at 120 degrees and the third at 240 degrees.
Drag each planet gear with the manipulator handle to confirm it rotates around its own axis. Adjust the mate connector angular offset if the teeth do not visually mesh with the sun and ring gears.

Aligning teeth by eye

If teeth overlap slightly, double-click the Revolute mate in the feature list to reopen it. Check Offset and rotate the part a few degrees until the teeth interleave cleanly with both the sun and ring gear teeth.

Planet gear not in the right position?

If a planet gear lands at the origin instead of at 22.5 mm, you may have selected the wrong mate connector. Double-click the mate and re-pick the second connector on the ring gear at the correct radius. Use the Measure tool to confirm the distance from center.

Help me position my planet gears correctly at 22.5 mm from center.

Add Gear Relations and animate

Mates define where parts can move. Relations define how mates interact with each other. A Gear Relation locks the rotation of two revolute mates to a constant ratio so that spinning one gear automatically spins the other at the correct speed.

In the Assembly toolbar, click the Relation icon (or find it in the toolbar menu).
In the Relation dialog, confirm Gear Relation is selected.
Select the sun gear's Revolute mate as the first mate.
Select the first planet gear's Revolute mate as the second mate.
The ratio is 1:1 because both gears have 15 teeth. Accept the relation.
Repeat this Gear Relation for the sun gear and each of the other two planet gears (1:1 ratio each time).

Why is the sun-to-planet ratio 1:1?

Gear ratio equals the number of teeth on the driven gear divided by the teeth on the driving gear. Both the sun and planet gears have 15 teeth, so 15/15 = 1:1.

Add another Gear Relation between each planet gear's Revolute mate and the ring gear. Since the ring gear is fixed, Onshape uses its implicit revolute degree of freedom.
Set the ratio to 1:3 (15 planet teeth to 45 ring teeth).
Accept each relation.

Now verify the whole mechanism works together.

Right-click the sun gear's Revolute mate in the feature list on the left.
Select Animate from the context menu.
Watch all three planet gears rotate around their own axes while the ring gear stays fixed.
If any teeth visibly intersect, stop the animation and adjust the angular offset on the offending Revolute mate (double-click the mate, check Offset, and rotate a few degrees).

What does Animate do?

The Animate command drives the assembly from a single mate's degree of freedom. All other mates and relations in the assembly are enforced simultaneously. This lets you verify that the entire gear train moves as a connected system.

Gears not rotating together?

If only the sun gear moves and the planets stay still, your Gear Relations may reference the wrong mates. Open each Relation in the feature list and confirm it links the correct Revolute mates (sun-to-planet, then planet-to-ring).

If you see a "relation only succeeds if the mates chosen are appropriate" warning, confirm both selected mates are Revolute type, not Fastened or Cylindrical.

Help me fix my Gear Relations so all planet gears rotate with the sun.

Verify together using Follow Mode

Both collaborators should see the final animation together to confirm the mechanism works before moving to export.

One person (Person A) navigates to the Planetary Assembly tab.
The other person (Person B) activates Follow Mode by double-clicking Person A's social cue icon in the toolbar at the top of the window.
Person B's workspace becomes outlined to indicate they are now following.
Person A right-clicks the sun gear's Revolute mate and selects Animate.
Both collaborators watch the planets orbit. Confirm no teeth visibly intersect at any point during rotation.
To stop following, Person B clicks anywhere in their browser window.

What does Follow Mode show?

Follow Mode mirrors the active tab, cursor movements, selections, and part movements in real time. Whoever is being followed controls what the follower sees, so both of you are watching the exact same animation simultaneously.

Don't see the other person's social cue icon?

The social cue icons only appear when both users are actively in the same document at the same time. Make sure both collaborators have the Planetary Gear Fidget document open in their browser.

Help me get Follow Mode working with my collaborator.

Your planetary gear mechanism is verified and ready to go. Next up, you will export STL files so you can 3D print a physical fidget toy at the library makerspace.

Export STL Files for 3D Printing

Your planetary gear assembly is verified and animating smoothly. The design lives inside Onshape, but your library makerspace's 3D printer needs a different file format to turn it into a physical object.

In this step, you will export each part as an STL file (the standard format for 3D printing), review print settings that keep gear teeth strong, and save a permanent version snapshot of your design.

In this step, get ready to:

Export all gear parts and housing as STL files.
Review print settings for gear tooth strength.
Save a permanent version snapshot of the design.

Export each part as an STL file

3D printers read STL files, which describe only the surface mesh of a part. You need one STL per part so the makerspace can print them individually.

Switch to the Sun and Planets Part Studio tab.
In the Parts list on the left, click the sun gear to select it.
Right-click the selected part and choose Export from the context menu.
In the Export dialog, set Format to STL.
Set Units to Millimeter.
Name the file sun-gear and click Export.
Repeat for one planet gear. Select a single planet gear in the Parts list, right-click, choose Export, keep the same STL/Millimeter settings, and name it planet-gear.

Why only one planet gear file?

All three planet gears are identical copies from the Circular Pattern. You only need one STL file. When you hand it to the makerspace, ask them to print 3 copies of planet-gear.stl.

Switch to the Ring and Housing Part Studio tab.
Select the ring gear body in the Parts list.
Right-click, choose Export, set Format to STL and Units to Millimeter, name it ring-gear, and click Export.
Select the top cap part, right-click, Export as STL in Millimeters, and name it top-cap.
Select the bottom cap part, right-click, Export as STL in Millimeters, and name it bottom-cap.

You should now have 5 STL files in your downloads folder: sun-gear.stl, planet-gear.stl, ring-gear.stl, top-cap.stl, and bottom-cap.stl.

Don't see all 5 files?

Make sure you exported from both Part Studio tabs. The sun gear and planet gear live in Sun and Planets, while the ring gear and caps live in Ring and Housing.

If a file downloaded with Onshape's default name instead of your chosen name, rename it in your downloads folder to match the naming convention above.

Help me troubleshoot my STL exports in Onshape.

Review print considerations for the makerspace

Before handing the files to the makerspace, you need to know the right print settings so your gear teeth come out strong and your parts fit together.

What print settings should I ask for?

Print orientation: all gears should print flat with the tooth face down. This avoids overhangs on the tooth profiles.
Layer height: 0.2 mm gives a good balance between speed and tooth accuracy.
Infill: 100% for gear teeth strength. The teeth are thin and need solid material to avoid snapping.
Supports: none needed. Spur gears printed flat have no overhangs.
Tolerance: the 0.1 mm backlash built into your design accommodates most FDM printers. Ask the makerspace staff what tolerance their printer typically achieves.

What if the gears are too tight or too loose?

If the makerspace printer runs slightly large, gears may be tight. If it runs small, gears may be loose. Either way, you can return to your Onshape document and adjust the Backlash variable in the Variable Studio, re-export, and reprint.

Create a version snapshot of your design

Onshape's version system lets you freeze the current state of your document. This creates a permanent, read-only snapshot so if either collaborator experiments later, you can always return to the print-ready state.

Look at the left edge of the Onshape interface for the Document panel (the vertical toolbar aligned with the Onshape logo).
Click the Create version icon in the Document panel.
In the dialog that appears, enter the name v1.0 - Ready for Print.
Click Create.

The new version now appears in the Versions and history panel. Both collaborators can see it.

What does a version do?

A version in Onshape captures the entire document state at that moment. It is immutable, meaning nobody can edit it. You remain in your active workspace and can keep designing, but the version stays frozen as a reference point you can always return to or branch from.

Can't find the Create version icon?

The Document panel is the vertical toolbar on the far left of the screen, aligned with the Onshape logo. The Create version icon is one of the icons in that panel. If you do not see it, try clicking the Versions and history icon in the same panel to open the history graph, then use the Create version icon at the top of that panel.

Help me find the Create version button in Onshape.

Secret mission

Convert to Herringbone Gears for Print-in-Place

What if you could print the entire planetary gear mechanism as a single piece with no assembly required? Herringbone (double-helix) teeth lock the gears axially so they cannot slide apart, making print-in-place possible. This challenge eliminates all post-print assembly by converting your design into one interlocking mechanism.

Clean Up Your Resources

Decide whether to keep your resources running, pause them to come back later, or delete them entirely. This project runs on the Onshape Free Plan and local files, so there are no ongoing costs.

Resources you used:

Onshape document Planetary Gear Fidget (shared, free plan, no cost).
STL files on your local machine (sun-gear.stl, planet-gear.stl, ring-gear.stl, top-cap.stl, bottom-cap.stl, planetary-print-in-place.stl).

Keep everything running

No action needed. Choose this if you plan to keep iterating on your design, experiment with different gear ratios, or share the document with others.

Your Onshape document persists indefinitely on the Free Plan at no cost.
Since Onshape Free documents are public, you can share the URL with anyone to show off your planetary gear design.
Your STL files remain on your local machine until you manually delete them.
Create additional Versions or Branches in Onshape to experiment with different tooth counts, gear ratios, or decorative features without affecting your print-ready version.

Pause - I'll come back to this later

There is nothing to pause for this project. Your Onshape document and local STL files remain available at no cost whether you use them or not.

Your v1.0 - Ready for Print Version snapshot in Onshape is permanent. You can always return to it even if you experiment further.
Bookmark the Onshape document URL so you can find it easily later.

Delete - I don't want to use this again

Remove all project resources and start fresh. Follow the steps below to delete everything.

Delete the Onshape document: go to the Onshape Documents page, right-click on Planetary Gear Fidget, and select Send to trash. Items in Trash are automatically deleted after 30 days on the Free Plan.
Delete your local STL files on macOS by running:
rm sun-gear.stl planet-gear.stl ring-gear.stl top-cap.stl bottom-cap.stl planetary-print-in-place.stl.
On Windows, open File Explorer, navigate to the folder where you saved the STL files, select all six files, and press the Delete key.
If you shared the document with your collaborator, they should also right-click it on their Documents page and select Send to trash to remove it from their account.

Nice Work!

Nice work! You and your dad just designed a complete planetary gear fidget toy from scratch in Onshape, ready to 3D print at your library makerspace.

You've learned how to:

Design a complete planetary gear set (sun gear, planet gears, ring gear, and housing) using parametric CAD and the Spur Gear FeatureScript to generate mathematically correct involute gear profiles.
Build a working assembly with revolute mates and gear relations that animates correctly, using Boolean subtraction to create the internal ring gear.
Collaborate in real-time with your dad using Onshape's simultaneous editing and Follow Mode, then export print-ready STL files and save a permanent Version snapshot.
Secret Mission: Converted to herringbone gears for a single-piece, print-in-place fidget toy that requires no assembly.

Ready to quiz yourself?