In this guide
The best first SOLIDWORKS projects are small parts you can measure: a drilled plate, a hollow spacer, an L-shaped bracket, a three-part assembly and a simple drawing. Each one teaches a specific skill, comes with a numerical check and includes a design change, so you learn how a model behaves rather than just copying clicks.
Key takeaways
- Start with simple geometry that has a clear purpose and a result you can calculate.
- Check every part with a measurement, such as volume or a known distance, before you add finishing touches.
- Practise revisions: change one dimension and predict the result before you rebuild.
- Move from parts to an assembly, then to a drawing, in that order.
- Keep your files organised and label practice work honestly in a portfolio.
Why do small first projects work better than impressive models?
Many beginners open SOLIDWORKS, search for a tutorial on a car wheel or a drone frame, and follow dozens of steps they do not understand. The finished model looks good, but if one dimension changes, the whole thing breaks and they cannot say why.
A small project with a clear brief avoids that trap. You know what the part should look like, you know its size, and you can check whether your model matches. When something goes wrong, there are only a few places to look.
The projects in this guide are original educational exercises. They are not official certification questions and they are not manufacturing-approved designs. All dimensions are in millimetres. They build in a sequence, from sketching and features to assemblies and drawings, and each one ends with a revision task.
That revision task matters more than it looks. In real engineering work, designs change constantly. A model that updates predictably when a dimension changes is far more useful than one that only looks right on the first attempt. This idea is called design intent, and these projects are built to teach it from the start.
If you are completely new to the interface, terms such as part, sketch, plane and feature may still be unfamiliar. The guide on the basics of SOLIDWORKS for beginners explains those foundations, and this article picks up where it leaves off with hands-on work.
What should you set up before your first project?
A little preparation saves a lot of confusion later. Before you draw a single line, sort out the following.
Units and templates
Set the document units to millimetres before entering any dimensions. A plate that should be 80 mm long becomes something very different if the template is set to inches. Check the units shown in the status bar each time you start a new document.
A project folder and clear filenames
Create one folder for these exercises and use descriptive names such as Plate_01, Spacer_01, Bracket_01 and Practice_Assembly. Assemblies refer to the part files they contain, so moving or renaming parts later can break those links.
A notebook or text file
Keep a short log of what you built, what went wrong and how you fixed it. This log becomes surprisingly valuable. It is also the start of an honest portfolio, because it shows your thinking rather than only the finished picture.
Software access
Use a properly licensed copy of SOLIDWORKS, whether through your school, your employer or a training provider. If you are joining a course, ask the course adviser how software access works for practice sessions.
Which first projects should you build, and in what order?
The table below shows the full project ladder. Each project adds one or two new skills while reusing what you learned before.
| Project | Main skills practised | How you check it | Revision task |
|---|---|---|---|
| 1. Drilled plate | Sketch, dimensions, extrude, cut | Volume calculation | Change the length |
| 2. Hollow spacer | Extrude versus revolve | Same volume from two methods | Change the outside diameter |
| 3. L-shaped bracket | Profile sketching, relations, feature order | Cross-section area and volume | Change one leg |
| 4. Three-part assembly | Inserting parts, mates | Measured pin projection | Change the spacer length |
| 5. Plate drawing | Views, dimensions, annotations | Someone else can rebuild the part from it | Update after a model change |
Work through them in order. Projects 1 and 2 give you the parts you need for Project 4, Project 3 teaches feature order, and Project 5 uses the plate from Project 1.
Project 1: How do you model and check a drilled plate?
Build a rectangular plate 80 mm long, 50 mm wide and 8 mm thick, with one 12 mm diameter hole through its centre. This teaches the most common pattern in mechanical modelling: a base feature followed by a cut.
- Open a new part and start a sketch on the Top Plane.
- Draw a centre rectangle with its centre on the origin.
- Dimension the rectangle to 80 mm by 50 mm and look at the sketch status. It should report that the sketch is fully defined.
- Extrude the rectangle 8 mm in one direction.
- Start a new sketch on the top face and draw a circle centred on the origin.
- Dimension the circle to a 12 mm diameter and use a Through All cut.
- Rename the features in the design tree, for example Base_Plate and Centre_Hole, then save.
Checking the plate
Use the Mass Properties tool to read the volume. The solid block is 80 × 50 × 8 = 32,000 mm³. The hole removes π × 6² × 8, about 904.78 mm³. The plate should therefore measure approximately 31,095.22 mm³.
If your number is far off, the usual causes are a radius of 12 mm entered instead of a diameter, the wrong document units, or a blind cut that did not go all the way through.
Revision task
Change the length from 80 mm to 100 mm. The hole should stay centred because it is tied to the origin, and the volume should rise by 20 × 50 × 8 = 8,000 mm³. Write one sentence explaining why the hole stayed in the middle. Then return the length to 80 mm, because you will use this plate in the assembly.
Project 2: How do you build a spacer two different ways?
Make a hollow cylindrical spacer with a 30 mm outside diameter, a 12 mm inside diameter and a length of 20 mm. The point is to compare two modelling methods that produce the same solid.
Method A: extrude a ring
On the Top Plane, sketch two circles centred on the origin, dimension them to 30 mm and 12 mm, and extrude the ring-shaped region 20 mm. Check that the middle is open and save the part as Spacer_01.
Method B: revolve a section
In a separate practice part, sketch on the Front Plane. Add a vertical centreline through the origin to act as the axis. Draw a rectangle entirely on one side of it, with its lower edge on the horizontal line through the origin. Place the inner edge 6 mm from the axis, the outer edge 15 mm from it, and make the rectangle 20 mm tall. Revolve it a full 360 degrees around the centreline.
Do not let the rectangle cross the axis. The values of 6 mm and 15 mm are radii, matching the 12 mm and 30 mm diameters. Mixing up radius and diameter is one of the most common reasons a beginner's spacer comes out twice the intended size.
Checking the spacer
Both versions should measure π × (15² − 6²) × 20, about 11,875.22 mm³. Matching results show that the feature you choose should follow the shape and the edits you expect later, not a belief that one command is always better.
Revision task
Increase the outside diameter to 34 mm in both versions, leaving the bore and length unchanged. Notice where each model stores that value: a circle diameter in Method A, a distance from the axis in Method B. Restore the original size before the assembly project.
Project 3: How does an angle bracket teach feature order?
Model a simple L-shaped bracket as one extruded profile. This is a shape exercise, not a sheet-metal part and not a load-rated support. The horizontal leg is 60 mm long, the vertical leg is 40 mm high, both are 6 mm thick, and the bracket is 30 mm wide.
On the Front Plane, connect these corner points in order and close the shape: (0, 0), (60, 0), (60, 6), (6, 6), (6, 40), (0, 40). The origin sits at the outside lower-left corner. Add horizontal and vertical relations and enough dimensions to fully define the outline, without duplicating any constraint.
Extrude the profile 30 mm.
Checking the bracket
The cross-section area is 60 × 6 for the horizontal leg plus 6 × 34 for the part of the vertical leg above it, giving 564 mm². The volume is 564 × 30 = 16,920 mm³.
Feature order
Save this plain version first. Then add a small fillet to an outside edge and watch the preview. Ask yourself which edges change and whether the fillet would still work if the leg became thinner. Keep cosmetic features such as fillets and chamfers near the end of the design tree, so the main dimensions stay easy to find and edit.
Revision task
Change the horizontal leg from 60 mm to 75 mm. The vertical leg, thickness and width should stay the same, and the volume should become 654 × 30 = 19,620 mm³. If a different dimension moves, fix the sketch relations rather than adding extra geometry to hide the problem.
Project 4: How do your parts become an assembly?
Now combine the original plate and spacer into a simple stack, held by a third part: a plain pin 12 mm in diameter and 35 mm long. Model the pin as a quick extruded circle. These are nominal training sizes. Equal pin and hole diameters do not describe a real manufacturing fit.
- Start a new assembly and insert the plate at the origin, so it becomes the fixed reference.
- Insert the spacer and add a concentric mate between its bore and the plate hole.
- Add a coincident mate between the spacer's lower face and the plate's upper face, checking the preview so it sits on top.
- Insert the pin and make it concentric with the plate hole.
- Make the pin's lower end face coincident with the plate's underside, so the pin points upward through the stack.
- Inspect the result with a section view.
Checking the assembly
The plate and spacer stack to 8 + 20 = 28 mm. With the pin starting at the underside of the plate, 35 − 28 = 7 mm should stick out above the spacer. Measure it.
Concentric and face mates can still leave the parts free to spin. For this symmetric exercise, that is acceptable. Avoid adding random mates just to lock every movement. Explain each relationship first, and if a mate fails, look at the existing mates before adding another.
Revision task
Change the spacer length to 24 mm and rebuild. The pin should now project 35 − (8 + 24) = 3 mm. If it does not, check whether the spacer still sits on the plate and whether the pin is still referenced to the plate underside.
Project 5: How do you turn a part into a useful drawing?
Create a drawing of the drilled plate with the standard orthographic views and an isometric view for orientation. Add the overall length, width, thickness, hole diameter and hole position. Pick a readable scale and state the units.
A good beginner drawing gives each dimension once, in the view where it reads most clearly. Repeating the same dimension in several views makes a drawing harder to read, not more complete.
The rebuild test
Give your drawing to a friend or classmate who has not seen your model and ask them to rebuild the plate from it. If they need to ask you a question, the drawing is missing something. This is one of the simplest and most honest checks a beginner can use.
Revision task
Change the plate length in the part file and open the drawing again. The views and dimensions should update. Practice dimensions like these are not a production specification: real manufacturing drawings also need material, tolerances and finish details chosen for the actual job.
How do you check mass, materials and shared files?
Volume checks need no material, but mass does. When an exercise gives a material, assign it from the material library and look at its density. Changing the appearance of a part does not change its engineering properties.
Watch the scope of the Mass Properties tool. If a face or component is selected, the result may only cover that selection. Clear any selection before recording a result for a whole part or assembly.
When you share an assembly, sending only the assembly file leaves out the parts it depends on. The Pack and Go tool collects the assembly and its referenced files into one folder or ZIP file. Open the packed copy from a different folder or computer to confirm it is complete.
What should you do when a model goes wrong?
Mistakes are part of learning, and a calm checking routine helps far more than starting again from scratch. Work through these questions in order.
- Units: are they still millimetres?
- Driving dimensions: does each value match the brief?
- Sketch relations: is the sketch fully defined, under defined or over defined?
- Feature settings: is a cut blind when it should go through all, or extruded in the wrong direction?
- References: after a change, which is the earliest feature showing an error?
- Assembly mates: which component is fixed, and do the mates describe what you intended?
If a sketch is over defined, find the conflicting relation instead of deleting constraints at random. Keep a copy of the file before trying a repair, and write a short note on the cause and the fix. A folder of understood mistakes teaches you more than a folder of unexplained finished models.
How can you practise in Dubai, in class or online?
Self-study with written briefs like these goes a long way, but feedback speeds things up. A trainer can look at your design tree and quickly spot a weak relation or a poor feature order, something that is hard to see on your own.
At Bright Future Training Institute, SOLIDWORKS training in Dubai runs in two formats.
| Option | Where it happens | Good fit for |
|---|---|---|
| Classroom | NBQ Building, Bank Street, Bur Dubai, close to BurJuman Metro Station | Learners who like working alongside a trainer and other students |
| Online live sessions | From home or the office, anywhere in the UAE | Working professionals and learners outside Bur Dubai |
The institute is open daily, 9:00 AM to 5:00 PM, and certificates are approved by KHDA and recognised across the UAE. You can book a free demo class before enrolling to see how sessions run. For fees, timings and how software access works, ask a course adviser, as these depend on the course and format you choose.
SOLIDWORKS sits alongside other design tools in the engineering courses range. If you are still deciding between mechanical and building design software, the comparison of SolidWorks versus Revit explains where each one fits.
Where do these projects lead next?
Once you can build all five projects from the written brief without a tutorial, you are ready for the next steps: patterns and mirrors, shells and ribs, more detailed drawings with sections and hole callouts, and larger assemblies.
Some learners then aim for a vendor certification. The guide to SOLIDWORKS certification and CSWA explains how that path works. Exam rules, fees and formats belong to the certification provider, so always confirm the current details on the official SOLIDWORKS certification website. A course certificate and a vendor certification are separate things.
For a portfolio, include a few original parts, a small assembly and a clear drawing, each with a short note on the checks and revisions you made. Label practice work honestly and keep the editable files, so you can show how each model responds to change.
Start building with guidance
Build these five projects slowly enough to understand every decision, then repeat them with new dimensions. If you would like a trainer to review your work, talk to a course adviser about SOLIDWORKS training in Bur Dubai or online, or book a free demo class. You can also reach the team on WhatsApp or phone at +971 54 373 3394, or by email at [email protected].