SolidWorks Tutorial - A Beginner Guide to SolidWorks

Dear reader,

We are proud to announce that we are launching our first premium SolidWorks tutorial. This tutorial is based on our own series of Lego Tutorial, but with greater in depth explanation. Instead of modelling those little piece of Lego, you will be modelling a more complex shape as you see on the left.

This tutorial consists of 5 chapters, where in every chapters different SolidWorks features is being introduced. A step by step explanation, complete with the screenshot, will guide you how to use each functions. Extrude, Revolve, Sweep, Loft, Mirror, are just a few of the functions that you will learn.

Priced at just US$15, you will get this 69-pages eBook in pdf format. This tutorial is a perfect investment to improve your SolidWorks skill.

So, what are you waiting for? Click on the "Buy Now" button to make the purchase. Or you could take a look at some of the preview below.
                    

A Beginner Guide to SolidWorks - Preview

Season Greeting & Important Announcement!

To all of our reader, we would like to wish all of you Merry Christmas and Happy New Year! Wish Santa bring you the gift of never ending happiness this Christmas!

On this Christmas season as well, we would like to announce that currently we are in the midst of preparing the first volume of our own SolidWorks tutorial. This tutorial will be a very useful guide for all of you who are new to SolidWorks and wanted to learn more about this software.

The tutorial will be based on our Lego Tutorial, with some modifications and update. Our initial Lego tutorial only teaches you the very basic function, which is Extrude Boss/Base and Assembly. The new tutorial would teach you how to use all SolidWorks basic functions, including Revolve, Loft, Sweep, as well as Pattern.

The tutorial tutorial would be released around mid of January 2015, so keep an eye on it! Please follow us to keep you updated!

SolidWorks Tutorial - Pen Cover

This time round, the tutorial I made would be to model one part of a pen, which is its cover. The complete set of assembly however, can be downloaded from here.

I chose to make the tutorial only for one part as you can learn how to use several features in this tutorial.

Skill learned: 

Revolved Boss/Base, Revolved Cut, Fillet, Sketch Relationship

Final Product:

Tutorial:

1. Open up SolidWorks > New > Parts.
2. On the Model Tree, right click on the Front Panel, and select Sketch.
   
3. Select the arrow besides line, and select Centerline. Draw a vertical line passing through the origin. 
   
4. Select line, and draw a shape of object that looks like shown below. 
   
5. Select Smart Dimension, and give the dimensions as shown below. Note that all dimensions against the Centerline are all for diameter, instead of radius. Read here for a note of how to give diameter instead of radius on revolve. 
   
   
   
   
6. Click Insert > Boss/Base > Revolve. Or alternatively, click on the Features Ribbon, and select Revolved Boss/Base. You should see a preview as shown below. Click the green thick button (OK) to confirm.
   
7. Right click on Front Plane, and select Sketch.
8. Repeat step 3, draw a vertical Centerline passing through the origin. Draw 6 rectangular box as shown below.
   
9. Hold down Ctrl button, and select all 6 inner edge of the rectangle. On the left dialog box, select Colinear and Equal.
   
10. Give the dimension of the rectangular box as shown below. Note that the spacing of the box (1.5 mm) is the same for all. 
    
11. Click Insert > Cut > Revolve. Or alternatively, click on the Features Ribbon and select Revolved Cut. A preview should appear. Select the green thick button (OK) to confirm. 
    
12. On the Features Ribbon, select Fillet. On the left dialog box, adjust the radius to 1 mm, and select the edge shown below. 
    
13. Add fillet on the edges of the revolved rectangle, adjust the radius to 0.1 mm and select all the edges as shown below. Note that you can select the surface (highlighted on the rightmost selection) instead of selecting the edges one by one. Read here for explanation of the selection.
    
14. Congratulation! You have completed your model!

Tutorial - Lego (2)

This tutorial is a continuation of the previous tutorial here. If you haven't completed the first part, it is advisable to complete the first part before doing this part.

In this part, now we're going to assemble few pieces of the Lego together to make some shape. After the completion of this tutorial, you can build your own 3D Lego!

1. Click File => New, and select Assembly.

2. The default setting for SolidWorks would automatically run the "Insert Components" feature. You can see it on the left side bar. Click on the "Browse" button, and locate the Lego piece you made in Part 1 of this tutorial. If you haven't closed it yet, it should appear on the "Open Documents" window above the "Browse" button. 

3. Now you should see your Lego piece displayed on the display window. Left click to confirm the placement of the piece. Now to insert another piece, click the "Insert Components" button located at the "Assembly" ribbon.

4. Same thing as step 3, left click anywhere to confirm the placement of your second Lego piece. You should see something like shown below.

5. After having two pieces together, now its time to arrange the placement of the pieces. Click on the "Mate" button located at the "Assembly" ribbon. You should see the Mate tab on the left side of the screen.

6. On the Mate tab on the left, select "Coincident" from the Standard Mates, and select the side of the first Lego pieces (Shown blue in figure below).

7. Now select the same side of the second piece. A pop-up box should appear after selecting the two surfaces. Click on the green thick button on the pop-up box.

8. Do the same thing as above, click Coincident, but now select the bottom surface of the the piece.

9. Then select the bottom surface of the second piece. Click the green thick on the pop-up box.

10. Same again, apply Coincident Mate (or some people call Constrain) on the two surfaces of the piece shown below. Click OK (green thick button) after that. Now your Lego piece should be arranged nicely, adjacent to each other. By now you should understand how to apply a simple Coincident mate according to your design intent.

11. Repeat step 3 and 4 to insert another piece of Lego.

12. Click on the Mate button. Now on the left side tab, click on the Concentric mate, and select the two cylindrical surface as shown below. 

13. Now give Coincident mate on the side surface of the piece as shown below.

14. Finally, give Coincident constrain on the top surface of the previous piece and the bottom surface of the third piece. Click OK to finalize the Mate.

15. Now you have completed the first series of tutorial to build a simple Lego assembly. You can have an experiment yourself to build a more complex Lego assembly :)

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.