Build a Desktop Catapult in Onshape

Collaboratively design and assemble a moving catapult using Onshape mates.

Introduction

30 Second Summary

Think about how products get designed in the real world. Engineers don't take turns passing a single file back and forth. They work on different parts at the same time, trusting that everything will fit together at the end.

In this project, you will team up with a partner to design and assemble a desktop catapult in Onshape. Each person builds different components simultaneously in the same document, then you bring everything together into a working assembly with moving parts.

What You'll Build

A multi-part desktop catapult with a base, uprights, trigger latch, rotating launch arm, axle, and projectile cup, all designed collaboratively in real time and assembled with motion-defining mates.

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

A shared Onshape Document with two Part Studios, one designed by each person at the same time.
A fully assembled catapult using Fastened mates (locking parts in place) and a Revolute mate (rotational motion).
An animated launch arm that swings within defined rotation limits, simulating the catapult firing.
Secret Mission: Add a crossbar brace and use Linear Pattern to create bolt holes in the base.

Are there any prerequisites?

Both participants need a free Onshape account (sign up at cad.onshape.com). You should also be comfortable with basic Onshape skills like creating sketches, extrusions, fillets, and chamfers.

Set Up Your Shared Document

Before you start sketching catapult parts, both participants need access to the same Onshape Document.

In this step, one person creates the shared document and invites the other. Then you'll each set up your own workspace so you can design different components at the same time without stepping on each other's work.

In this step, get ready to:

Create and share a new Onshape Document called "Desktop Catapult."
Create two Part Studio tabs, one for each person.
Confirm you can see each other's presence in the document.

Create and share the Desktop Catapult document

One person (Person A) creates the document and shares it. The other person (Person B) accepts the invitation and opens it in their browser.

Person A: On the Onshape Documents page, click Create in the top left.
Select Document from the menu.
Name the document Desktop Catapult and click Create.
Once the document opens, click the Share button on the Document toolbar (top right area, near your avatar).
Enter Person B's email address in the share dialog.
Set the permission to Can edit.
Click Share to send the invitation.
Person B: Check your email for the Onshape invitation and click the link to open the document. Alternatively, find it on your Documents page under documents shared with you.
Both people should now have the document open in their browsers. Look for each other's colored avatar circles at the top of the document to confirm you're both present.

What are social cues?

The colored circles at the top of an Onshape document are called social cues. They indicate which collaborators are currently in the document and which tab or feature they're working on.

You'll rely on these throughout the project to stay aware of what your partner is doing.

Why is my document public?

On the Onshape Free plan, all documents are public by default. Anyone with an Onshape account can view and copy your document, but only people you explicitly share with at the Can edit level can make changes. This is fine for a learning project.

Don't see each other's avatars?

Make sure both people have the same document open (not just the Documents page). The colored circles only appear when both collaborators are inside the document at the same time.

If Person B cannot find the document, confirm the sharing email arrived and that Person A entered the correct email address in the Share dialog.

Why can't my partner see the document I shared?

Create the Part Studio tabs

Each person gets their own Part Studio to work in. This avoids feature tree conflicts and mirrors how real engineering teams split component ownership.

Person A: Click the + tab at the bottom of the document window.
Select Part Studio.
Rename the new tab to Base and Uprights by double-clicking its tab name and typing the new name.
Person B: Click the + tab at the bottom of the document window.
Select Part Studio.
Rename the new tab to Arm and Cup.

Both people should now see two Part Studio tabs at the bottom of the document.

Why two Part Studios instead of one?

Onshape supports multiple parts in a single Part Studio, but using separate Part Studios (one per person) avoids feature tree conflicts during simultaneous editing.

This mirrors real-world workflows where different engineers own different components. It also naturally teaches the Insert workflow you'll use later when assembling everything together.

Don't see the + tab?

The + button sits at the far right of the tab bar at the bottom of the screen. If you cannot see it, try widening your browser window or scrolling the tab bar to the right.

If Person B sees a greyed-out + or gets an error, confirm that Person A shared the document with Can edit permission (not Can view).

Help me fix my Part Studio tab permissions

Confirm real-time collaboration is active

Person A: Click on your Base and Uprights tab to open it.
Person B: Click on your Arm and Cup tab to open it.
Look at the tab bar at the bottom. You should see your partner's colored avatar appear on the tab they're working in.

This confirms Onshape's simultaneous editing is active. Any changes either person makes will appear in real time for the other.

Use Follow Mode to watch your partner

Double-click your partner's colored avatar circle at the top of the document to enter Follow Mode. You'll see their cursor and exactly what they're looking at. Click in white space or another tab to exit.

Your shared workspace is ready. Next up, you'll split the work. Person A designs the base, uprights, and trigger latch while Person B builds the launch arm, axle, and cup.

Person A Designs the Base, Uprights, and Trigger Latch

Your shared document is ready, and both participants can see each other working in real time. Now it is time to build the catapult's foundation.

Person A will design the base plate, two upright supports, and a trigger latch. These parts form the structural frame that holds the launch arm in place and catches it in the loaded position.

In this step, get ready to:

Sketch and extrude a base plate with filleted edges and two tall uprights with axle holes.
Model a trigger latch with an L-shaped hook profile that will catch the arm.
Communicate the interface dimension to Person B using an Onshape Comment.

Sketch and extrude the base plate and uprights

The base plate is the catapult's footprint. The uprights rise from it to hold the axle that the arm pivots on.

Person A, switch to the Base and Uprights Part Studio tab at the bottom of the document.
Click the Sketch tool in the Feature toolbar at the top.
Select the Top plane as your sketch plane.
Draw a Corner rectangle and dimension it to 100mm wide by 60mm deep.
Click the green checkmark to accept the sketch.
Click Extrude in the Feature toolbar.
Set the depth to 8mm and make sure the direction arrow points upward.
Keep the operation set to New and click the checkmark to accept.
Select the Fillet tool from the Feature toolbar.
Click all four top edges of the base plate.
Set the fillet radius to 3mm and click the checkmark.

You should see a flat rectangular slab with softly rounded top edges.

Why start with the base plate?

The base anchors the entire catapult assembly. By building it first, you create reference surfaces that the uprights and trigger latch can attach to.

Now add the two uprights that will hold the axle.

Click the top face of the base plate to select it.
Click Sketch to start a new sketch on that face.
Draw two rectangles, each 10mm x 15mm.
Position them symmetrically so their centers are 30mm apart and 20mm from the front edge of the base.
Accept the sketch with the green checkmark.
Click Extrude and set the operation to New so each upright becomes its own part.
Set the depth to 50mm upward and click the checkmark.
Select the Chamfer tool from the Feature toolbar.
Click the top edges of both uprights.
Set the chamfer distance to 2mm and click the checkmark.

You now have two tall rectangular columns rising from the base with angled top edges.

Finally, cut the axle holes through both uprights.

Click the inner face of one upright (the face facing the other upright).
Click Sketch to start a new sketch on that face.
Draw a circle with a diameter of 8mm.
Position the circle's center 40mm above the top surface of the base plate.
Accept the sketch.
Click Extrude and change the operation type to Remove.
Set the End type to Through all so the hole passes completely through the upright.
Click the checkmark to accept.
Repeat the same process on the second upright: sketch an 8mm circle at the same height (40mm from the base top), extrude with Remove and Through all.

What does Remove do in the Extrude dialog?

When you set the Extrude operation to Remove, Onshape subtracts material instead of adding it. This is how you create holes and cuts in existing parts.

Setting the End type to Through all ensures the cut passes completely through the part, regardless of thickness.

Both uprights should now have clean circular holes at the same height. These holes will hold the axle that Person B is designing.

Hole not going all the way through?

Make sure you selected Remove (not New) as the operation type. Also confirm the End type is set to Through all rather than Blind.

If the hole created a separate floating cylinder instead of cutting, undo with Ctrl+Z (Windows) or Cmd+Z (macOS), then re-extrude with Remove selected. Why is my extrude creating a new part instead of cutting a hole?

Design the trigger latch

The trigger latch is a small L-shaped hook that catches the arm when it is pulled back into the loaded position. When the arm swings forward, it releases off the hook.

On the inner face of one upright, about 10mm below the axle hole, click to select that face.
Click Sketch to start a new sketch on that face.
Draw an L-shaped profile: a vertical leg that is 3mm wide and 12mm tall.
At the top of the vertical leg, extend a horizontal hook that reaches 6mm inward (toward the center of the catapult).
Accept the sketch with the green checkmark.
Click Extrude with the operation set to New.
Set the depth to 5mm and click the checkmark.
Select the Fillet tool.
Click the inner corner where the vertical leg meets the horizontal hook.
Set the fillet radius to 1mm and click the checkmark.

You should see a small ledge protruding from the inner face of the upright. The rounded inner corner allows the arm to release smoothly when it swings forward.

Why add a fillet to the hook corner?

A sharp 90-degree corner would catch the arm and prevent it from releasing cleanly. The 1mm fillet creates a smooth transition that lets the arm slide off the hook when it swings past the latch.

L-shape not extruding as expected?

Make sure your sketch profile is fully enclosed (no gaps between lines). Open sketch lines will not form a valid extrude region.

If Onshape highlights the wrong region, click the correct enclosed area in the Extrude dialog to select it manually. Help me fix my L-shaped sketch so it extrudes correctly.

Agree on the interface dimension with your partner

Your trigger latch has a 6mm horizontal hook. Person B needs to design a matching notch on the arm that catches on this hook.

Right-click on the trigger latch extrude feature in the Feature list on the left side of the screen.
Select Add comment from the context menu.
Type a message confirming the interface dimension, for example: "The arm needs a 6mm x 3mm notch on its underside to catch on this hook. Position it about 15mm from the pivot hole."
Click Add to post the comment.

A comment icon appears next to the feature in the Feature list. Person B receives a notification and can read the exact dimensions they need to match.

Why communicate dimensions through Onshape Comments?

In real collaborative CAD work, parts designed by different people must fit together at shared interfaces. Embedding the agreed dimensions directly on the relevant feature keeps the information next to the geometry it describes.

This prevents miscommunication that would cause parts to not fit during assembly. The comment is tied to the feature, so anyone reviewing the design later can see the coordination decision.

Person B can switch to this tab at any time and see your design taking shape in real time.

Your catapult frame is complete. Next up, Person B builds the launch arm, axle, and projectile cup that will slot into the holes you just created.

Person B Designs the Arm, Axle, and Cup

While Person A builds the base and frame, Person B focuses on the moving parts. The arm, axle, and cup are the mechanical heart of the catapult.

In this step, Person B creates three parts that interface with Person A's uprights through the axle holes. Getting the dimensions right (especially the 8mm pivot hole matching Person A's upright holes and the 7.8mm axle diameter for slight clearance) ensures a smooth assembly later.

In this step, get ready to:

Sketch and extrude the launch arm with a pivot hole and trigger notch.
Create a cylindrical axle sized to fit Person A's upright holes.
Model a shelled cup on the arm to hold the projectile.

Sketch and extrude the launch arm

The launch arm is the longest part of the catapult. It needs a pivot hole near one end (where the axle passes through) and a small notch on the underside that catches on Person A's trigger latch.

In the Arm and Cup Part Studio, click the Sketch tool in the Feature toolbar.
Select the Front plane as your sketch plane.
Draw a rectangle using the Corner rectangle tool. Set it to 120mm wide and 10mm tall.
Click the green checkmark to accept the sketch.
Click Extrude in the Feature toolbar.
Set the Operation to New and enter a depth of 8mm.
Click the green checkmark to accept the extrude.

What does this create?

You now have a flat beam that is 120mm long, 10mm wide, and 8mm thick. This is the launch arm that will pivot between Person A's uprights.

Next, add the pivot hole so the axle can pass through the arm.

Start a new sketch on one of the flat (8mm x 10mm) end faces of the arm. Choose the face that is 25mm from one end. This end becomes the pivot end.
Draw a circle using the Center point circle tool. Set the diameter to 8mm and center it on the arm face, 25mm from the pivot end.
Accept the sketch with the green checkmark.
Click Extrude and set the Operation to Remove.
Set the End type to Through all so the hole passes completely through the arm.
Click the green checkmark to accept.

Why 8mm for the hole?

Person A's uprights have 8mm diameter axle holes. The arm's pivot hole matches this diameter so the axle can pass through all three parts (upright, arm, upright) in a straight line.

Now add the trigger notch on the underside of the arm. This notch catches on Person A's 6mm trigger latch hook.

Start a new sketch on the underside (bottom face) of the arm, near the pivot end.
Draw a small rectangle 6mm wide and 3mm deep, positioned about 15mm from the pivot hole center.
Accept the sketch.
Click Extrude and set the Operation to Remove.
Set the depth to 3mm (or use Through all if your sketch is already constrained to 3mm).
Click the green checkmark to accept.

Why 6mm for the notch?

Person A confirmed via an Onshape Comment that the trigger latch hook extends 6mm inward. Your notch matches this dimension so the arm catches securely on the latch when pulled back into the loaded position.

You should now see a flat beam with a circular through-hole near one end and a small rectangular notch cut into the underside.

Don't see the hole or notch?

Make sure the Extrude Operation is set to Remove, not New or Add. The Remove operation cuts material away from the existing arm.

If you see an error, check that your sketch circle or rectangle is fully within the arm's face. The sketch region must fall entirely within the target geometry for the Remove extrude to succeed.

Help me troubleshoot my Remove extrude not cutting through my arm in Onshape.

Create the axle

The axle is a simple cylinder that passes through both of Person A's upright holes and through the arm's pivot hole. Its diameter is slightly smaller than 8mm to allow rotation.

Click the Sketch tool and select the Right plane as your sketch plane.
Draw a circle using the Center point circle tool. Set the diameter to 7.8mm.
Accept the sketch with the green checkmark.
Click Extrude and set the Operation to New.
Enter a depth of 50mm. This length spans both uprights (which are 30mm apart) with extra material on each side.
Click the green checkmark to accept.

Why 7.8mm instead of 8mm?

The 0.2mm clearance between the 7.8mm axle and the 8mm holes allows the arm to rotate freely around the axle. Without this clearance, the parts would be a press-fit and would not move during assembly animation.

You should see a new cylinder in your Part Studio, separate from the arm beam. The Parts list on the left should now show two parts.

Axle merged with the arm?

If you only see one part in your Parts list, the axle may have been added to the arm instead of created as a new part. Double-click the Extrude feature in the Feature list to edit it. Make sure the Operation is set to New, not Add.

Help me separate my axle from my arm in Onshape.

Model the projectile cup

The cup sits on the opposite end of the arm from the pivot hole. You will create a solid cylinder and then use the Shell feature to hollow it out, leaving walls of consistent thickness.

Start a new sketch on the top face of the arm, at the end opposite the pivot hole (the far end).
Draw a circle using the Center point circle tool. Set the diameter to 20mm and center it on the arm face.
Accept the sketch.
Click Extrude and set the Operation to New.
Enter a depth of 15mm extruding upward from the arm surface.
Click the green checkmark to accept.

Now hollow out the cup using the Shell feature.

Click the Shell tool in the Feature toolbar.
Click the top face of the cylinder (the flat circular face at the top). This is the face that will be removed to create the opening.
In the Shell thickness field, enter 3mm.
Click the green checkmark to accept the shell.

What is the Shell feature?

The Shell feature removes material from a part to produce a cavity with constant wall thickness. You select one or more faces to remove, and Onshape hollows out the interior while keeping walls at your specified thickness.

In this case, removing the top face creates an open cup shape. The 3mm walls are thick enough to hold a small projectile without looking paper-thin.

Your Part Studio should now show three distinct parts in the Parts list: the arm beam, the axle cylinder, and the hollow cup.

Shell not working?

Make sure you are selecting the top face of the cup cylinder, not the entire part. The Shell tool requires you to click the face to remove in the Faces to shell field.

If you accidentally select the wrong face, click on the selected face again to deselect it, then click the correct top face.

Help me use the Shell feature to hollow out my cup in Onshape.

Use Follow Mode to watch Person A

Double-click on Person A's colored avatar circle at the top of the document to enter Follow Mode. You will see their cursor and their view of the model in real time. Click in white space or switch to another tab to exit Follow Mode.

Person B's parts are complete. Both participants can now switch to each other's Part Studio tabs at any time to inspect the parts. Next, you will both come together to assemble the full catapult using mates.

Assemble the Catapult Together

Both halves of your catapult now exist in separate Part Studios. Person A has built a sturdy base with uprights and a trigger latch. Person B has a launch arm, axle, and cup ready to go.

Now you will bring everything into a single Assembly and connect the parts using mates. Mates define how parts relate to each other and whether they can move.

In this step, get ready to:

Create an Assembly tab and insert all parts from both Part Studios.
Fix the base and apply Fastened mates to lock stationary parts together.
Add a Revolute mate to give the launch arm rotational motion around the axle.

Person A creates the Assembly and inserts base parts

The Assembly is where all your separate parts come together and get positioned relative to each other. Person A will create this tab and bring in the base components first.

Person A clicks the + tab at the bottom of the document.
Select Assembly.
Name the Assembly Catapult Assembly and press Enter to confirm.
Click Insert in the Assembly toolbar.
In the Insert dialog, select the Base and Uprights Part Studio.
Click on the base plate, both uprights, and the trigger latch to place them all into the Assembly workspace.
Click the green checkmark to close the Insert dialog.

Why do all the parts appear floating?

When parts are first inserted, they have all six degrees of freedom (3 translation, 3 rotation). They are completely free to move until you fix or mate them. Your next job is to anchor one part as the stationary reference.

In the Instances list on the left side, right-click the base plate.
Select Fix.

What does Fix do?

Fix removes all degrees of freedom from the base plate, anchoring it as the ground reference. All other parts will be positioned relative to it. A small pin icon appears next to the base in the Instances list to confirm it is fixed.

Now lock the trigger latch to the upright. Since Person A modeled the latch in position on the upright's inner face, the two parts already overlap correctly. A Fastened mate locks them together with zero degrees of freedom.

Click the Mate tool in the Assembly toolbar (or press M).
Hover over the trigger latch where it touches the upright until a small dot (mate connector) appears. Click to select it.
Hover over the upright's inner face at the same location and click the mate connector that appears there.
In the Mate dialog, confirm the type is set to Fastened.
Click the green checkmark to apply the mate.

What are mate connectors?

Mate connectors are local coordinate systems that appear as small dots on faces and edges when you hover during mate creation. They define the exact point and orientation where two parts connect. Onshape uses these as the basis for all mates.

Person B should be able to switch to the Catapult Assembly tab at any time and see the base components appearing in real time.

Person B inserts arm parts and mates the cup

Person B now adds their components to the same Assembly. Both people will see all parts together in the workspace for the first time.

Person B clicks on the Catapult Assembly tab at the bottom of the document.
Click Insert in the Assembly toolbar.
Select the Arm and Cup Part Studio.
Click on the arm, axle, and cup to place them all into the Assembly.
Click the green checkmark to close the Insert dialog.

Both participants can now see all parts floating in space together. Person B will attach the cup to the arm using a Fastened mate.

Person B clicks the Mate tool (or presses M).
Hover over the bottom face of the cup and click the mate connector at its center.
Hover over the top face of the arm at the cup end (the end far from the pivot hole) and click the mate connector there.
Confirm the mate type is set to Fastened.
Click the green checkmark to apply.

Why Fastened for the cup?

The cup should never move relative to the arm. A Fastened mate restricts all degrees of freedom (0 DOF), bonding the two parts together as if they were welded. The cup will move only when the arm moves.

Parts snapping to the wrong position?

If the cup flips upside down or lands on the wrong face, the mate connectors' axes may be misaligned. Double-click the mate in the Mate Features list to edit it. Use Flip Primary Axis or Reorient Secondary Axis to correct the orientation, then click the green checkmark again.

Help me fix a mate that positioned my part incorrectly.

Add the key mates together

This is the most important part of the assembly. You will add a Revolute mate that lets the arm rotate around the axle, then lock the axle into both uprights so the whole mechanism holds together.

Click the Mate tool (or press M).
Hover over the cylindrical face of the axle until a mate connector appears at its center. Click to select it.
Hover over the inside of one upright's axle hole until a mate connector appears at the hole center. Click to select it.
In the Mate dialog, change the type from Fastened to Revolute using the dropdown.
Click the green checkmark to apply the Revolute mate.

What does a Revolute mate do?

A Revolute mate provides one degree of freedom: rotation about the Z axis. The axle can spin in the upright's hole, but it cannot slide or shift in any other direction. This is exactly the behavior you want for a pivot point.

Now lock the arm onto the axle so they rotate together.

Click the Mate tool again.
Select a mate connector at the center of the arm's pivot hole (the 8mm hole 25mm from one end).
Select a mate connector on the axle's cylindrical face at the same position.
Confirm the type is set to Fastened and click the green checkmark.

Finally, lock the axle into the second upright so it cannot slide out.

Click the Mate tool one more time.
Select a mate connector on the axle's end face or cylindrical surface near the second upright.
Select a mate connector at the center of the second upright's axle hole.
Confirm the type is set to Fastened and click the green checkmark.

Use Solve if parts look misaligned

If previously added mates become unsolved after adding new ones, click the Solve button in the Mate dialog. This regenerates all mates and repositions parts correctly.

Time to test the motion. Click and drag the arm in the Assembly workspace. It should rotate smoothly around the axle between the two uprights.

Click anywhere on the arm and drag it up and down.
Confirm the arm swings in an arc around the axle pivot point.
Visually check that the trigger notch on the underside of the arm lines up with the latch hook when the arm is pulled back into the cocked position.

Arm not rotating?

If the arm stays locked in place, you may have accidentally used a Fastened mate instead of Revolute for the axle-to-upright connection. Double-click that mate in the Mate Features list and change the type to Revolute using the dropdown.

If the arm rotates but the trigger notch does not align with the latch, the arm may be flipped. Edit the Fastened mate between the arm's pivot hole and the axle, then use Flip Primary Axis to correct the arm's orientation.

Help me debug why my catapult arm is not rotating correctly.

Your catapult is fully assembled and moving. Next up, you will animate the arm's rotation and add motion limits to restrict it to a realistic launch arc.

Animate and Verify the Motion

Your catapult is fully assembled and the arm rotates freely on its axle. The next question is: does it move the way a real catapult should?

In this step, you will animate the Revolute mate to watch the arm swing, add rotation limits so it stays within a realistic range, and save a permanent snapshot of the completed design.

In this step, get ready to:

Animate the Revolute mate in Reciprocate mode to see the arm swing back and forth.
Add motion limits to restrict the arm to a 0-90 degree range.
Save a Version to preserve the completed catapult design.

Animate the Revolute mate

The Animate command drives a single mate through its degrees of freedom so you can watch the assembly move without manually dragging parts.

In the Catapult Assembly tab, find the Revolute mate in the Mate Features list on the left side of the screen.
Right-click the Revolute mate and select Animate.
In the Animate dialog, set the Playback type to Reciprocate.
Leave the Steps value at the default for now.
Click the Play icon to start the animation.

You should see the catapult arm swing continuously back and forth around the axle.

What does Reciprocate mode do?

Reciprocate plays the animation from the start value to the end value, then reverses back, repeating continuously until you manually stop it.

The Steps value controls animation speed. A lower value produces a faster animation, and a higher value produces a slower one.

Try adjusting the Steps value up or down to see how it changes the speed of the arm's swing.
Click the Stop icon to halt the animation when you are satisfied.

Arm not moving?

Make sure you right-clicked the Revolute mate specifically. Fastened mates have zero degrees of freedom and cannot be animated.

If the Animate option is grayed out, check that you are clicking the mate in the Mate Features list (not the part instance).

Why can't I animate my Revolute mate?

Add motion limits to the Revolute mate

Without limits, the arm can spin a full 360 degrees around the axle. A real catapult arm stops when it hits the uprights, so you need to restrict the rotation range.

Double-click the Revolute mate in the Mate Features list to open its editing dialog.
Check the Limits box to enable motion limits.
Set the minimum rotation to 0 degrees.
Set the maximum rotation to 90 degrees.
Click the green checkmark to accept the changes.

Why 0 to 90 degrees?

This restricts the arm so it cannot swing past the uprights. Zero degrees represents the resting (cocked) position, and 90 degrees represents the fully launched position where the arm is upright.

When limits are defined on a mate, the Animate feature automatically uses them as the start and end values for the animation range.

Right-click the Revolute mate again and select Animate.
Confirm the Start value and End value are now populated with 0 and 90 respectively.
Set Playback type to Reciprocate and click Play.

The arm should now swing smoothly between 0 and 90 degrees and reverse, staying within the uprights the entire time.

Arm still spinning past the uprights?

Make sure you checked the Limits box and not just the Offset box. They are separate options in the Revolute mate dialog.

Double-click the mate to re-open it and verify both the minimum and maximum values are entered.

Help me fix my Revolute mate limits

Save a Version of the completed design

A Version in Onshape is an immutable snapshot of the entire document at a specific point in time. Once created, its geometric data cannot be changed.

Click the Create version icon in the Document panel (next to the document name at the top of the screen).
In the name field, type Version 1 - Complete Catapult.
Click Create.

The new version appears in the Versions and history panel. You remain in the active workspace and can continue editing freely.

What is a Version in Onshape?

Versions are moments in time that cannot be changed. They capture every Part Studio, Assembly, and tab in the document exactly as they were at creation.

This means both of you can always return to this snapshot regardless of future edits. Think of it like a permanent save point in a game.

Verify the version was saved by clicking the Versions and history icon on the left side of the graphics area.
You should see Version 1 - Complete Catapult listed in the history graph alongside the default Start version.

Don't see the Create version icon?

The icon is located in the Document panel area near the document name at the very top of the interface. It is not in the feature toolbar.

You can also access version creation through the Versions and history panel on the left side of the graphics area.

Help me find the Create version button in Onshape

Secret mission

Add a Crossbar and Bolt-Hole Pattern

Your catapult works, but real engineering demands structural rigidity and mounting points. Can you add a crossbar brace between the uprights and use Linear Pattern to efficiently stamp bolt holes into the base?

Clean Up Your Resources

Decide whether to keep your resources running, pause them to come back later, or delete them entirely. This project runs entirely on Onshape's cloud (Free plan), so there are no ongoing costs.

Resources you used:

Onshape Document: "Desktop Catapult" (stored on Onshape's cloud, public on the Free plan).
Onshape Free accounts (one per participant).

Keep everything running

No action needed. Choose this if you're still actively building or plan to revisit the catapult design soon.

Your "Desktop Catapult" document stays on Onshape's cloud indefinitely at no cost.
Both participants retain edit access to the shared document.
On the Free plan, all documents are public. Anyone with the link can view your catapult.
Your Onshape Free accounts remain active with no time limit and no charges.

Pause - I'll come back to this later

There is nothing to pause for this project. Onshape Free documents persist on the cloud at no cost whether you use them or not.

Close the browser tab. Your document is saved automatically.
When you're ready to return, sign in at cad.onshape.com and open the "Desktop Catapult" document from your Documents page.

Delete - I don't want to use this again

Remove all project resources permanently. Only the document owner (Person A) can delete the document.

Delete the Onshape Document:
Remove Person B from the shared document (if not deleting it outright): Person B can right-click the document on their Documents page and select Remove to unsubscribe from the shared document.
Delete your Onshape Free account (optional, per participant):

Nice Work!

Nice work! You and your partner just designed and assembled a fully interactive desktop catapult in Onshape, working on different parts at the same time in the same document.

You've learned how to:

Design interrelated parts simultaneously in separate Part Studios, coordinating shared dimensions through Onshape Comments and real-time presence cues.
Assemble a multi-part mechanism using Fastened mates (0 DOF) to lock parts in place and a Revolute mate (1 DOF) to create rotational motion around an axis.
Animated assembly motion with rotation limits and saved an immutable Version to preserve your completed design state.
Secret Mission: Added structural reinforcement with a crossbar brace and used Linear Pattern to efficiently replicate bolt holes across the base plate.

Ready to quiz yourself?