Design a Desk Caddy in Onshape

Collaboratively design and assemble a two-part desk caddy using parametric CAD.

Introduction

30 Second Summary

Designing a product with another person usually means emailing files back and forth, hoping you're both working on the right version. Real engineering teams solve this by working in the same design tool at the same time.

In this project, you will design a two-part desk caddy collaboratively in real time using Onshape, a browser-based 3D CAD tool. One person designs a pen cup, the other designs a phone stand, and you assemble both parts into a finished product together.

What You'll Build

A two-part desk caddy designed collaboratively in Onshape, where each person sketches, constrains, extrudes, and fillets their own part before assembling them into a single unit.

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

A pen cup and phone/card stand designed simultaneously in the same shared document.
A fully assembled desk caddy with parts that fit together via agreed-upon dimensions.
Hands-on experience with the core parametric CAD workflow: sketch, constrain, extrude, fillet, and assemble.
Secret Mission: Design a connector bridge with chamfered edges that locks both parts together.

Are there any prerequisites?

None. This guide walks you through creating free Onshape accounts and setting up your shared document from scratch. All you need is a computer with a browser.

Set Up Onshape Accounts and Create a Shared Document

To design a desk caddy together, you and your collaborator need a shared workspace where both of you can model in real time.

Onshape is a browser-based CAD tool that works like Google Docs for 3D modeling. In this step, you'll both create free accounts and set up a shared document so you can design simultaneously.

In this step, get ready to:

Create Onshape Free accounts for both collaborators.
Set up a shared document with edit permissions.
Agree on the critical shared dimension that connects both parts.

Create Onshape Free accounts

Both you and your collaborator need separate Onshape accounts. Each account requires a unique email address.

On both laptops, open Google Chrome and navigate to cad.onshape.com.
Click Sign up in the top right corner.
Fill in the required information (name, email, password) and click Get Started.
Use a different email address for each account.

What happens after you sign up?

Onshape sends an activation email to each address. Click the Activate your account button in the email to verify your account and set up your sign-in credentials.

On first sign-in, Onshape asks you to set default units (Length, Angle, Mechanical) and runs a browser check. Accept the defaults and click Next, then Done.

Check your email inbox for the activation message from Onshape.
Click Activate your account in the email.
Set a password, accept the terms of service, and click Get started.
Complete the default units setup and browser check by clicking Next and then Done.
When prompted, set a display Nickname. This is what your collaborator sees as your avatar label in the document.

Don't see the activation email?

Check your spam or junk folder. The email comes from Onshape (a PTC company). If it still hasn't arrived after a few minutes, return to cad.onshape.com and try signing in with the email you used. Onshape may prompt you to resend the activation.

Help me troubleshoot my Onshape account activation.

After activation, both of you should land on the Onshape Documents page. This is your home base for all documents.

Create a shared document and invite your collaborator

One person creates the project document and shares it with the other. It doesn't matter who does this step.

One person clicks the blue Create button in the top left corner of the Documents page.
Select Document... from the dropdown menu.
Type Desk Caddy Project as the document name.
Click OK (or press Enter) to create the document.

The document opens with two tabs at the bottom of the screen: Part Studio 1 (where you build individual parts) and Assembly 1 (where you combine them later).

Click the Share button in the top right of the document toolbar.
In the Share dialog, type your collaborator's email address into the email field.
Set the permission dropdown to Can edit.
Click Share.

What does Can edit mean?

The Can edit permission gives your collaborator the ability to edit, copy, export, share, and comment on the document. Both of you can work in the same Part Studio simultaneously, and all changes appear in real time.

Your collaborator opens their Onshape Documents page.
Click the Shared with me filter in the left sidebar to find the document.
Click Desk Caddy Project to open it.
Confirm you can both see each other's avatar in the top right area of the document. This indicates real-time collaboration is active.

Your documents are public on the Free plan

All documents created on the Onshape Free plan are publicly visible to other Onshape users. No one can edit your document without explicit permission, but they can view and copy it. This is fine for a learning project.

Can't see each other's avatar?

Make sure both of you have the same document open (not just the Documents page). The collaborator avatar only appears when both users are inside the same document at the same time. Try refreshing the browser if the avatar doesn't appear within a few seconds.

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

Agree on shared dimensions

In real engineering teams, components designed by different people must fit together at their connection points. Before building anything, you need to agree on the dimension that both parts share.

Agree with your collaborator that both parts will have a base width of 60mm. This shared edge is what lets the parts sit flush when assembled.

Why agree on 60mm?

When two people design parts that must connect, they need at least one shared measurement. The 60mm width acts as the interface between your pen cup and phone stand. Without this agreement, the parts would be different sizes and wouldn't align in the assembly.

This is exactly how professional engineering teams work. Teams define interface dimensions before building, so each person can design independently while knowing the parts will fit.

Take a moment to explore the interface together. Notice the Part Studio 1 tab at the bottom (where you build individual parts).
Notice the Assembly 1 tab (where you combine parts later).
Look at the Feature toolbar along the top of the screen. This is where you'll find tools like Sketch, Extrude, and Fillet.
Notice the Feature list panel on the left side. Every modeling action you take appears here as a history entry.

What is a Part Studio vs an Assembly?

A Part Studio is where you design individual 3D parts from scratch using sketches and features. You can have multiple Part Studios in one document.

An Assembly is where you bring finished parts together and define how they connect. Think of Part Studios as workshops for building individual pieces, and the Assembly as the table where you put them all together.

Your collaborative workspace is ready. Next up, you'll each design your own part. Person A will build the pen cup, and Person B will build the phone stand.

Design the Pen Cup (Person A)

Your shared document is ready and both collaborators can see each other working in real time. Now it's time to build the first physical component of the desk caddy.

Person A will design a pen cup in Part Studio 1. This is a hollow open-topped box with rounded edges, sized to hold pens and pencils upright on your desk.

Who works where?

Person A stays in Part Studio 1 for this step. Person B should skip ahead to Step 3 and work simultaneously in a new Part Studio they create.

Both of you will be editing the same Onshape document at the same time. You can see each other's changes appear live as you work.

In this step, get ready to:

Sketch a 60mm x 80mm rectangle as the cup's base profile.
Extrude the sketch into a solid block and hollow it out with Shell.
Add fillets to round off the sharp edges.

Sketch the pen cup base

Every 3D part in Onshape starts as a 2D sketch. You draw a flat shape on a plane and lock its size with dimensional constraints before turning it into a 3D object.

In Part Studio 1, click the Sketch button in the toolbar.
Select the Top plane as your sketch surface.
Click the Center point rectangle tool in the sketch toolbar.
Click on the origin point (the small dot at the center) and drag outward to draw a rectangle. Don't worry about the exact size yet.
Press D on your keyboard to activate the Dimension tool.
Click the horizontal (bottom) edge of the rectangle and type 60. Press Enter.
Click the vertical (side) edge of the rectangle and type 80. Press Enter.
Click the green checkmark to accept the sketch.

What are dimensional constraints?

When you add a dimension in Onshape, you lock that measurement in place. The sketch lines turn from blue (under-constrained) to black (fully constrained) once all dimensions are set.

Your 60mm width is the shared dimension that both parts use. This ensures the pen cup and phone stand will line up perfectly when assembled side-by-side.

Your sketch should now show a black rectangle centered on the origin, labeled 60 and 80.

Rectangle not showing the right dimensions?

Make sure you clicked the edge itself (not a corner point) when adding each dimension.
If you accidentally set the wrong value, double-click the dimension number in the sketch to edit it.
If you can't find the Dimension tool, press D on your keyboard as a shortcut.

Help me fix my sketch dimensions in Onshape.

Extrude and hollow the cup

Extrude turns your flat 2D sketch into a 3D solid by pulling it upward. Shell then scoops out the inside, leaving thin walls and an open top.

Click Extrude in the Feature toolbar.
The sketch region should auto-select (it appears shaded gray). If not, click the rectangle area in the sketch.
In the Extrude dialog, set the depth to 100. Press Enter.
Click the green checkmark to create the solid block.

You should see a solid rectangular block on screen. It is 60mm wide, 80mm deep, and 100mm tall.

Click Shell in the Feature toolbar. If you don't see it, click the dropdown arrows in the toolbar's tool groups to reveal additional tools.
Click the top face of the block (the large flat face on top).
Set the wall thickness to 3.
Click the green checkmark.

What does Shell do?

Shell removes the interior of a solid part, leaving walls of a uniform thickness. By selecting the top face, you told Onshape to leave that face open.

The result is a box you can drop pens into. The 3mm walls are thick enough to be structurally sound while leaving plenty of room inside.

Your block is now a hollow cup with 3mm thick walls and an open top.

Shell didn't work as expected?

Make sure you selected only the top face. If you selected a side face, the wrong surface will be open.
If you see an error, undo with Cmd+Z (macOS) or Ctrl+Z (Windows) and try again.
Double-check that the thickness is set to 3, not 30 or 0.3.

Help me fix my Shell feature in Onshape.

Add fillets to soften the edges

Fillets replace sharp edges with smooth rounded curves. They make parts look more polished and feel comfortable to handle.

Click Fillet in the Feature toolbar.
Select the 4 vertical outer edges of the cup (the tall corner edges). Hold Shift to select multiple edges.
Set the radius to 5.
Click the green checkmark.

The four tall corners of your cup are now smoothly rounded.

Click Fillet again in the Feature toolbar.
Select the 4 bottom outer edges of the cup (where the base meets the sides).
Set the radius to 2.
Click the green checkmark.

Why two separate fillet operations?

Different edges serve different purposes. The large 5mm fillets on the vertical edges give the cup a modern, rounded appearance.

The smaller 2mm fillets on the bottom edges add a subtle professional touch without changing the cup's silhouette dramatically.

Your pen cup is complete. Check the Feature list on the left side of the screen.

You should see five features listed: Sketch 1, Extrude 1, Shell 1, Fillet 1, and Fillet 2.

Fillet showing an error?

If you get a failure, the radius might be too large for the remaining geometry. Make sure you used 5 for vertical edges and 2 for bottom edges, not the other way around.
Confirm you selected outer edges, not inner edges. The inner edges are inside the hollow cup.
If an edge won't select, try rotating the view (two-finger drag on trackpad) to click it from a different angle.

Help me fix my Fillet feature in Onshape.

✔️ Awesome, I've got everything!

Great. Double check that your Feature list shows all five features in order before moving on.

ⓧ I'd like to double check the full feature list

Your Feature list on the left should contain these five features in this exact order:

Sketch 1 - A 60mm x 80mm center point rectangle on the Top plane.
Extrude 1 - 100mm depth, creating the solid block.
Shell 1 - 3mm wall thickness with the top face removed.
Fillet 1 - 5mm radius on the 4 vertical outer edges.
Fillet 2 - 2mm radius on the 4 bottom outer edges.

If any feature is missing or shows a red error icon, right-click it in the Feature list and select Edit to adjust its settings.

Your pen cup is ready. Next up, Person B designs the phone and card stand in their own Part Studio.

Design the Phone/Card Stand (Person B)

Person A is working on (or has already finished) the pen cup in Part Studio 1. Now it is Person B's turn to create the second half of the desk caddy.

You will design a phone and card stand with a flat base and an angled back support. The critical constraint is that your base must be exactly 60mm wide to match Person A's pen cup, so both parts slot together flush in the final assembly.

In this step, get ready to:

Sketch and dimension the stand base to match the shared 60mm width.
Extrude a base platform and an angled back support.
Apply fillets for smooth, professional edges.

Create a new Part Studio for your part

Each person works in their own Part Studio so you can model simultaneously without interfering with each other's features.

At the bottom of the screen, click the + tab.
Select Create Part Studio.
Right-click the new tab at the bottom and rename it to Phone Stand.

Why a separate Part Studio?

In Onshape, Part Studios are independent design environments within the same document. Each Part Studio has its own feature history.

By working in separate Part Studios, you and Person A can sketch and extrude at the same time without your features conflicting.

You should now see a blank Part Studio tab labelled Phone Stand at the bottom of your screen, next to Part Studio 1 and Assembly 1.

Sketch the stand base

The base is a flat rectangle that matches the pen cup's 60mm width. This shared dimension is what makes the two parts fit together in the assembly.

Click Sketch in the Feature toolbar at the top.
Select the Top plane as your sketch surface.
Select the Center point rectangle tool from the sketch toolbar.
Click the origin point, then drag outward to draw a rectangle centered on the origin.
Press D to activate the Dimension tool.
Click the horizontal edge and type 60. Press Enter. This is the shared 60mm width.
Click the vertical edge and type 50. Press Enter. The base is now 60mm x 50mm.
Click the green checkmark to accept the sketch.

What did I just do?

You created a fully constrained 2D rectangle on the Top plane. The dimensions lock the shape so it cannot accidentally resize. The 60mm width matches Person A's pen cup exactly, which is what allows the two parts to sit flush when assembled.

The green checkmark confirms and closes the sketch, making it available for 3D features like Extrude.

Sketch showing red or orange lines?

Red lines mean the sketch is over-constrained (too many dimensions). Orange lines mean it is under-constrained (not enough dimensions). Make sure you have exactly two dimensions: 60mm on the horizontal edge and 50mm on the vertical edge.

help me fix my sketch constraints

Extrude the base and add an angled back

The stand has two distinct shapes: a flat base platform and a tall angled back that leans to hold a phone or business card upright.

Click Extrude in the Feature toolbar.
The sketch region should auto-select (shaded gray). Set depth to 15 (15mm thick base platform).
Click the green checkmark to accept.

You now have a solid 15mm thick base. Next you will sketch the angled back support on the Right plane.

Click Sketch and select the Right plane as your sketch surface.
Select the Line tool from the sketch toolbar.
Draw 4 lines to form a closed trapezoid shape for the back support. The shape should be 15mm wide at the bottom (matching the base thickness), 3mm wide at the top, and 70mm tall.
Connect the lines so all 4 corners meet and form a closed shape.
Press D to activate the Dimension tool.
Click the bottom edge of the trapezoid and type 15 to lock the bottom width. Press Enter.
Click the top edge and type 3 to set the top width. Press Enter.
Click one of the vertical or angled sides and type 70 to lock in the height. Press Enter.
Click the green checkmark to accept the sketch.

Why a trapezoid?

The trapezoid creates a tapered back support. It is thick at the bottom (15mm, matching the base) for structural strength and thin at the top (3mm) so a phone or card leans at a comfortable angle.

This shape is a common approach in product design for creating stable angled supports.

Click Extrude in the Feature toolbar.
The trapezoid region should auto-select. Set the depth to 60 (the full 60mm width).
Check the Symmetric checkbox in the Extrude dialog. This extrudes equally from both sides of the Right plane, centering the back support on the base.
Click the green checkmark to accept.

What does Symmetric do?

The Symmetric option extrudes out from both sides of the selected plane equally. Since the sketch is on the Right plane (which passes through the center of the base), checking Symmetric pushes 30mm to the left and 30mm to the right for a total width of 60mm.

Without Symmetric, the extrusion would go 60mm in one direction only, leaving the back support offset to one side of the base.

Back support not centered on the base?

Make sure you checked Symmetric in the Extrude dialog before clicking the checkmark. If you forgot, double-click the Extrude feature in the Feature list on the left to re-open its settings and enable Symmetric.

help me fix my symmetric extrusion

Fillet the stand for comfort and aesthetics

Fillets round off sharp edges. On a phone stand, the top edge is where the phone rests, so a smooth fillet prevents scratching.

Click Fillet in the Feature toolbar.
Select the top edges of the angled back support (the thin edges at the 70mm height).
Set the radius to 3 (3mm) for a smooth phone-resting edge.
Click the green checkmark to accept.

Click Fillet again in the Feature toolbar.
Select the bottom edges where the angled back meets the base platform.
Set the radius to 4 (4mm) to create a strong-looking transition.
Click the green checkmark to accept.

Why two different fillet sizes?

The 3mm fillet on top gives a gentle curve where the phone rests. The 4mm fillet at the base creates a smooth structural transition between the back and the platform.

Different radii serve different purposes: comfort on top, visual strength on the bottom.

Rotate your view (two-finger drag on the trackpad to orbit, pinch to zoom) to inspect the part from all angles. You should see a flat base with an angled back rising from it, all edges smoothly rounded.

Fillet failing or showing an error?

Fillets can fail if the radius is too large for the edge geometry. Make sure you are selecting edges (not faces) and that the radius does not exceed the shortest adjacent face dimension. For the top edges, 3mm should work. For the bottom transition edges, 4mm should work.

help me fix a failed fillet

✔️ My stand looks complete

Your Feature list on the left should show these features in order: Sketch 1, Extrude 1, Sketch 2, Extrude 2, Fillet 1, and Fillet 2. The part is a 60mm x 50mm flat base with a 70mm tall tapered back support.

ⓧ Something looks off

Double-check your Feature list on the left side panel. You should have exactly 6 features:

Sketch 1 (60x50mm rectangle on the Top plane).
Extrude 1 (15mm base platform).
Sketch 2 (trapezoid on the Right plane: 15mm bottom, 3mm top, 70mm tall).
Extrude 2 (60mm Symmetric, creating the angled back).
Fillet 1 (3mm on the top edges of the back support).
Fillet 2 (4mm on the bottom edges where the back meets the base).

If any feature is missing or shows a red error icon, double-click it in the Feature list to edit its settings. Check that dimensions and edge selections match the values above.

Both parts now exist in the same Onshape document in separate Part Studios. Next up, you and Person A will bring them together in the Assembly tab and mate them side-by-side into a finished desk caddy.

Assemble the Desk Caddy Together

Both parts are designed and ready to meet. The whole point of agreeing on that 60mm shared width is about to pay off.

In this step, you'll bring both parts into the Assembly tab and connect them using a Fastened mate. This locks the parts flush along their shared edge, forming the final desk caddy.

In this step, get ready to:

Insert both parts into the Assembly tab.
Fasten the parts side-by-side using a mate.
Verify the fit, measure dimensions, and customize part colors.

Insert both parts into the assembly

The Assembly tab is where individual parts come together into a finished product. You'll insert each part from its Part Studio, and Onshape will automatically fix the first one in place as your anchor.

Click Insert in the Assembly toolbar at the top of the screen.
In the Insert dialog, you will see both Part Studios listed under Current document.
Click the pen cup part from Part Studio 1.
Click the green checkmark to place it in the assembly.

Why is the pen cup fixed in place?

The first part inserted into an Onshape Assembly is automatically fixed at the origin. This gives the assembly a stable anchor point. All other parts you insert will move relative to this fixed part when you apply mates.

Click Insert again in the toolbar.
Select the phone stand part from the Phone Stand Part Studio.
Click the green checkmark to place it roughly near the pen cup.

Both parts now appear in the assembly, but the phone stand is floating freely. You should see both parts in the 3D view and listed in the Instances panel on the left.

Don't see both Part Studios in the Insert dialog?

Make sure you're selecting from the Current document tab in the Insert dialog. Both Part Studios exist in the same shared document and should appear automatically.

If you only see one Part Studio, confirm that both you and your collaborator saved your Part Studios by clicking the green checkmark on any open features before switching to the Assembly tab.

help me find my parts in the Insert dialog

Mate the parts side-by-side

Mates define how parts connect to each other in an assembly. The Fastened mate removes all degrees of freedom between two surfaces, locking them together so they cannot move relative to each other.

Click the mate dropdown in the Assembly toolbar (look for Fastened, Revolute, and Slider as the first three mate types).
Select Fastened.
For the first mate connector, hover over the pen cup until you see small dots appear on its faces. Click the flat side face of the pen cup (the 80mm x 100mm face where you want the stand to attach).
For the second mate connector, click the matching flat side face of the phone stand (the 50mm x 70mm face).
The parts snap together, sharing their 60mm edges flush.
Click the green checkmark to accept the mate.

What are mate connectors?

When you hover over a face in the Assembly, small dots appear. These are locations where Onshape can create mate connectors. Each connector acts as a coordinate system with its own x, y, and z axes. Onshape uses these points to align parts precisely when you apply a mate.

Parts snapped together in the wrong orientation?

If the parts are overlapping or facing the wrong direction, look for the Flip Primary Axis or Rotate Secondary Axes icons in the Mate dialog. These let you adjust the orientation without re-selecting faces.

You can also delete the mate (right-click it in the Instances list and select Delete) and try again, clicking a different dot on the face to change the alignment point.

help me fix my mate orientation

Verify the assembly and explore together

Your desk caddy is now assembled. Time to inspect it from all angles and add some visual polish so you can tell the parts apart at a glance.

Rotate the view by using a two-finger drag on your trackpad to orbit around the assembly. Pinch to zoom in and out.
Click your collaborator's avatar at the top of the screen to activate Follow mode. This lets you watch their view in real time.
Click the Measure tool in the toolbar to confirm dimensions. Click an edge of the assembled caddy to verify the total width matches your expectations.

What does the Measure tool show?

The Measure tool displays measurement information about edges and faces. Click any edge to see its length, or click two faces to see the distance between them. Use this to confirm the pen cup's 60mm side is perfectly flush with the phone stand's 60mm side.

Right-click the pen cup in the 3D view.
Select Edit appearance from the context menu.
Choose a color from the color picker, then click the green checkmark to apply it.
Right-click the phone stand and repeat the process with a different color.

Your assembly now shows two distinctly colored parts sitting side-by-side with their 60mm edges perfectly aligned.

Try different viewing angles together

Take turns activating Follow mode to share your perspective with your collaborator. Orbit around to the back, top, and bottom of the assembly. This is how engineering teams review designs before manufacturing.

Parts don't appear flush?

Double-click the Fastened mate in the Instances list on the left to reopen its dialog. Check that both mate connectors are on the correct faces. If needed, delete the mate and reapply it, making sure you select the flat side faces (not the top or bottom faces) of each part.

help me align my parts flush in the assembly

Your desk caddy is assembled and looking great. Next up, you'll tackle the Secret Mission and design a connector bridge that ties both parts together with a brand new CAD feature.

Secret mission

Design a Connector Bridge

Your desk caddy has two parts sitting side-by-side. Can you design a third piece that bridges across the top of both, locking them together visually? This challenge introduces the Chamfer feature and the Extrude Remove workflow.

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 in the browser on Onshape's Free plan, so there are no ongoing costs.

Resources you used:

Onshape document "Desk Caddy Project" (stored on Onshape's cloud, publicly visible to other Onshape users).
Two Onshape Free accounts (one for each collaborator).

Keep everything running

No action needed. Choose this if you want to revisit or iterate on your desk caddy design later.

Your Onshape Free accounts remain active indefinitely at no cost.
The "Desk Caddy Project" document stays in your Documents page and remains publicly visible to other Onshape users (this is a Free plan limitation).
You can return to the document any time by signing in at cad.onshape.com.

Pause - I'll come back to this later

Since Onshape Free has no ongoing costs, pausing simply means signing out. Your document and accounts remain safe in the cloud until you return.

Click your Account user icon in the top-right corner and select Sign out.
Your collaborator should do the same on their browser.
When you are ready to return, sign back in at cad.onshape.com and your document will appear on the Documents page.

Delete - I don't want to use this again

Remove the project document and optionally delete both Onshape accounts entirely.

Delete the document:

The person who created the document (the owner) must perform this step. Click the Onshape logo in the top-left corner to return to the Documents page.
Find "Desk Caddy Project" in the document list. Right-click the document and select Send to trash.
To permanently delete it, click the Trash filter in the left sidebar, then click Empty trash. Items in Trash are automatically deleted after 30 days if you skip this step.
The collaborator who was shared on the document does not need to do anything. Once the owner deletes it, the document disappears from their "Shared with me" list.

Delete your Onshape accounts (optional):

Click your Account user icon in the top-right corner and select My account.
Click the Profile tab.
At the bottom of the page, click Delete my account.
Read the confirmation modal carefully. Type delete my account and enter your password to confirm.
Your account and all associated data will be deleted within 30 days. This action is not recoverable.
Both collaborators should repeat these steps on their own accounts if they wish to delete.

Why delete is optional

Onshape Free accounts cost nothing and have no time limit. Keeping your account lets you revisit your design, explore Onshape's Learning Center, or start new projects. There is no financial reason to delete.

Nice Work!

You and your dad just designed a complete two-part desk caddy together in Onshape. From empty Part Studios to a fully assembled 3D model, you experienced the same collaborative parametric CAD workflow used by professional engineering teams around the world.

You learned how to:

Designed individual 3D parts using the core parametric CAD workflow: sketch, constrain, extrude, shell, and fillet.
Assembled multiple parts using Fasten mates with proper alignment on shared 60mm dimensions.
Experienced real-time collaboration by simultaneously designing in the same Onshape document and seeing each other's changes live.
Secret Mission: Designed a connector bridge introducing the Chamfer feature and Extrude Remove workflow.

Ready to quiz yourself?