Tutorial - Lego (1)

For those who are totally new to SolidWorks, this tutorial might help you to learn to do your first model. What you need is just a little bit of effort to do follow every steps carefully.

This is going to be a 2-series tutorial, where in the first post you'll make the lego piece (part) and at the second part of the tutorial you'll assemble the lego pieces together (assembly).

1. Open up SolidWorks on your computer. After it loaded, a screen like below should be seen.

2. Click File => New => Parts. A display as shown below should be seen. Note on the model tree (left tab), a default front, top, and right plane and the origin is automatically created.

3. Right click on the "Top Plane", and choose sketch (on the left side of the glasses logo).  By doing this, you're going to create a 2D sketch on the top plane.

4. After doing step no. 3, you will notice that the ribbon on top is now automatically set to "Sketch" ribbon. Press spacebar, and select "Normal To". Notice that now the top plane is now aligned to your computer screen. Choose the rectangular icon from the ribbon, and draw arbitrary rectangular as shown below.

5. Now click on "Smart Dimension" from the sketch ribbon. Click on the top line on the left followed by line on the right, and enter 24 mm for the value. This step is used to give dimension to the sketches. Give all dimension to all the lines so that it look like what is shown in figure below. Note that all the line has turned from blue to black color.

6. After completing the sketch, now its time to extrude the sketch. Click insert => Boss/base => Extrude (Alternatively, you can click on Features tab and click Boss Extrude). Notice that Boss extrude tab now appears on the left side of the screen. Select Blind on the drop down menu of Direction 1, and enter the value of 10 mm. See image below for reference. After all these have been done, click on the green thick button (lets call it OK button) to confirm the feature. Now you have a solid block =)

7. Now click on the top surface of the solid (shown in blue in image below), right click on it, and select Sketch.

8. Press space bar, and choose Normal to, such that that surface is now facing you. Draw two circle, randomly, like shown below. Left click on the left circle. While holding ctrl button, left click on the right circle. On the left tab (Properties), select equal.

Note: Holding the ctrl button allows you to do multiple selection.
By adding equal relations on the two circles, now they will have same radius.

9. Now select the center of the left circle.

10. While holding ctrl button on your keyboard, select the center of the right circle. On the left tab (Properties), select Horizontal. Observe that now the two circle is aligned horizontally.

11. On Sketch Ribbon, click on Smart Dimension and give dimension to the circle as shown below. Notice after giving all these dimensions, the circle color should change from blue to black.

12. Same like previously, now we need to extrude the circle (See step 6 if you forget how to extrude). On the left tab, Select Blond and extrude for 5 mm. Click the OK button to confirm. The shape of the LEGO piece started to form.

13. Now select the bottom face (shown in blue in image below). Right click and select "sketch".

14. Draw a random rectangular and using the "Smart Dimension", give a dimension as shown in picture below.

15. Now select Insert => Cut => Extrude. On the Cut Extrude tab on the left side, select blind with a distance of 9 mm.

16. You should see the result as something like shown below.

Now, select the inner surface as shown below in blue, right click, and select Sketch. 

17. Same step as previously, draw four circles (two of them to be concentric to each other), and give dimensions as shown below. Note that I started to skip few details as you should have done previously.

18. Click Insert => Boss/base => Extrude. On the Boss Extrude tab on the left side, select "Up To Surface" for direction 1, and select the pink surface shown in image below as the reference surface.

19. Now select the surface as shown below in blue, right click, and select sketch.

20. Draw a random rectangle and give dimension as shown in image below.

21. Draw two circles, concentric to the circle we extruded previously like shown below (shown in blue color). Alternative method is to use "Convert Entities", and select the outer edge of the circles.

22. Now from the Sketch ribbon, select "Trim Entities", and select "Power Trim" from the Trim option tab on the left side. Left click on the mouse, hold, and drag the cursor through the unwanted part of the sketch as shown in image below.

Note: This step, how to use Trim, is a very important step. Make sure you understand how to use the Trim tool.

23. Likewise, do the same thing on the unwanted part of the sketch on the right side.

24. Using the same technique as step 18, perform an Boss Extrude, Up To Surface, and the pink surface shown below as the reference surface.

25. Now do the same thing, sketch two vertical rectangles and using Smart Dimension, complete the sketch as shown below.

26. Using Trim tool, trim away unwanted sketch like shown in image below.

27. Similarly, perform Up To Surface Boss Extrude until the bottom surface of the Lego piece. If you follow all the steps correctly, you should have a rough shape of a Lego piece like shown below. Now what is left is just some finishing to make it look more realistic =)

28. Click Insert => Features => Chamfer. On the Chamfer options box on the left side, enter 1 mm for the chamfer distance and the angle to be 45 degree (default is set at 45 deg), and select all four outer corners of the Lego piece. Click OK to finalize the feature.

29. Using the same setting, insert another chamfer at all four inner corner of the piece.


30. Click OK to finalize and create the chamfer. Now your Lego piece should look something shown below. You're almost reaching the end =)

31. Insert chamfer again, but this time enter 0.30 mm for the chamfer distance, leave the angle at default 45 degree. Select the top and bottom edges of the Lego piece (shown in dotted blue line in image below). Click OK to proceed.

32. Now you have reached the end of the first tutorial part. Your Lego piece should look like the real Lego piece as shown below. Congratulation on your completion!

Continue to the second part of the tutorial here.

SolidWorks - Assembly

An assembly is a combination of parts or another assemblies together. You can read the basic of assembly here.

Insert Components

As the name said, the "Insert Components" is used to place parts or other assemblies in the assembly. When you first start your assembly, SolidWorks would automatically execute this function to prompt you to insert a component. To place your desired component, simply click on the Browse button to locate the file you wish to insert inside.

You can see how the scree would look like when you start an assembly. Note that now you have "Assembly" ribbon on top. To access this function again in future, simply click on the "Insert Components" function on the Assembly ribbon or from the drop down menu, click Insert => Component => Existing Part/Assembly.

Mate

Mate is used to define the location and how each parts relate to each other. Mate can be accessed easily from the Assembly ribbon or from the drop down menu, click Insert => Mate.

In SolidWorks, the mate is divided into three categories, Standard Mate, Advanced Mate, and Mechanical Mate. For most application , Standard Mate would be sufficient to fully defined an assembly. Advanced Mate and Mechanical Mate is used more for doing simulation.

Moving Components

To move components (parts or assembly) in the assembly, you can simply left click on the component and drag it to where you want to move. To rotate the component, change it to right click and drag it along. 

For more precise movement, you can use the "Move Component" function that can be accessed from the Assembly ribbon or from drop down menu, click Tools => Component => Move for moving component; or Tools => Component => Rotate, for more precise rotation.

When you have mate between components, the relationship between the two components defined by the mate would still be maintained when you move the components. This capabilities is not available in all CAD system that makes SolidWorks one of the best software for quick design as it is very good at simulating how each components relate when it is moving relative to each other.

SolidWorkds - Sweep

Sweep is a common feature in most of the CAD software to produce a solid. As mentioned before (see here), to make the sweep feature, you would need a "sweep profile" and a "sweep path". In SolidWorks, the sweep path need not coincide the sweep profile.

Compared to other CAD software, SolidWorks sweep feature offers a lot additional options.

Options

The first options on the feature shown is very useful for creating twisting solid. For demonstration, you could see the picture below. The shown solid is created by choosing "Twist Along Path" for 3 turns.

Guide Curves

Guide curve function allows you to have the sweeping profile to follow the guide curve in addition to following the sweeping path. User can select more than one guide curves to create complex solids.

Start/End Tangency

The Start/End tangency allow you to have the starting or ending profile of the swept solid to be tangential to either the sweeping path or another specified directional vector.

Thin Feature

Same like extrude and revolve, sweep function also allow user to have thin-feature option to make a hollow solid.

Gallery - Range Rover Classic

The Range Rover Classic is the second car I model after the Nissan 370Z Fairlady. Compared to my first car model, I feel that this is a much better model. Having much more details, all the surfaces are smooth, no abrupt transition between adjacent surfaces. Took me around a month to complete (averaging two hours per day).

The main assembly itself consists of:

• The body shell (including all the doors and windows)
• Wheel (the tire and the rim)
• Headlights and fog-lights.

Not a very realistic assembly tree (I need much more powerful computer to make realistic assembly tree!), but nonetheless, it looks quite a like the real thing though =)

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UPDATE

Further project, I would like to make the assembly looks more real, Probably to separate the side mirror with the body shell assembly so that I can have it folded =)

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The full assembly - shown with the guide curves and sketches.

Head light, fog light, and front grill.

The wheel - one part that I think really look alike the actual one.

Front air intake

Side mirror - Still in one piece with the body shell.

Gallery - Watch

This model was amongst my first few models when I was learning CAD modeling. Was done using SolidWorks, All the components are  created by Extrude and Revolve function only.

The biggest challenge of this model is that the chain that is not exactly flat, but at some certain radius. Nevertheless, it could be done using a simple revolve cut.

If you are interested to download the raw files, you can download it here.

The hook - not that easy to model a fully functioning hook

Overall Assembly

One of the most difficult section to model back then.

The other end

Back-side of the chain

SolidWorks - Revolve

Same like the extrude function, the revolve function is also divided into two category, the Revolved Boss/Base and Cut-Revolve. To understand the basic operation of revolve function and the difference between boss and cut, refer here.

Accessing the Function
Similar like the extrude function, you could access the revolve function from the ribbon.

Alternatively, you can go to Insert > Boss/Base > Revolve for Revolved Boss/Base. For Revolved Cut, you can click Insert > Cut > Revolve.

Revolved Options

Just like Extrude function, the Revolve function also has few options. The interface of the function is shown in picture below.

Revolve Type

Under Revolve-Type option, there are few options could be chosen, which are Blind, Up To Vertex, Up To Surface, Offset From Surface, and Mid Plane. By default, it is set to Blind. All these options has its own advantages, depending on its application.

Thin Feature

Just like Extrude, you can also have Thin Feature option on Revolve. The Thin-Feature option would create an offset to the selected profile. The offset distance is determined by the user. Thin-feature is extremely useful for doing a piping modeling.

The effect of Thin-Feature is seen in figure below, where a revolve angle of 270 degree, Thin-Feature with offset distance of 5 mm is determined by the user. The result would be a 3/4 revolution of hollow pipe.

Selected Contours

When there are more than one closed loop contours, user can choose which contours they wish to revolve. This works the same way as Selected Contours in Extrude function.