101 solidworks 3d sketch

free solidworks tutorial-3d-sketch

type : tutorial ebook - PDF

whats in for audience: lesson to exercise solidworks 3d-sketch

target feature of tutotrial: solidworks 3d-sketch

features used in tutorial:

  • solidworks 3d-sketch
  • solidworks fillet
  • solidworks refrence geometry
  • solidworks sweep
  • solidworks mirror
  • solidworks  linear pattern

difficulty level: advanced

provided by: SolidWorksAdvisor (SWA)

price: free solidworks tutorial PDF book

 

 

download the solidworks tutorial in pdf

download the solidworks model

or read the tutorial here:

solidworks tutorial-3d-sketch

we will create this frame during the tutorial :

1 101 solidworks 3dsketch tutorial

In this tutorial I assume that you know the basic of solidworks and you should know how to interactively work with the software . if you don’t know the basics I recommend you to visit the solidworks beginner tutorial first.

What we use to accomplish this model :

  • 3d sketch
  • Line
  • Circle
  • Fillet
  • Smart dimension
  • Plane
  • Swept boss/base
  • Mirror
  • Liner pattern 

As its name complies , 3d sketch is all about creating sketches in three dimensions . Usually when we are sketching in 2d , we are working on one of standard planes (XY ,XZ , ZY ) but in 3d sketching you can switch between these planes when you are drawing .

Solidworks offers two kinds of 3d sketching , you can sketch along any direction in 3d space (3d sketching) or you can make separated sketches in different planes in just one single sketch (3d sketching with planes) . Our model here is about 3d sketching .

Talking about 3d sketching can be confusing so let’s go ahead and experience it .

Open a new solidworks part . click on the “sketch” tab . Mouse over the little triangle on the sketch button and click it 

2 101 solidworks 3dsketch tutorial

now you are in 3d sketching environment . click on line . your mouse pointer changes , a pencil with XY . it means that if you draw a line it will be on XY plane . press tab once and your pointer changes to YZ , press it once again and it changes to ZX . this way you can switch between sketching planes . red arrows on the origin also show you which plane you are drawing on .

switch to YZ plane by pressing tab key then click on the origin . drag the mouse in the direction of Z axis (the little z in the yellow coordinate indicates that you are in the direction of z axis) and click again . just draw a line . you will dimension it later .

3 101 solidworks 3dsketch tutorial

Don’t exit the line . press tab once to switch to XZ plane and draw a line in x direction .

4 101 solidworks 3dsketch tutorial

Press tab and sketch along Y and click again .

5 101 solidworks 3dsketch tutorial

Exit the line . now your sketch must be like this :

6 101 solidworks 3dsketch tutorial

Select the line again and click on the last point. Sketch a line like this in the XY plane .

7 101 solidworks 3dsketch tutorial

That’s it . just use the tab key to get the right plane and direction . continue the line and draw two more lines to get the final sketch like bellow :

8 101 solidworks 3dsketch tutorial

Now dimension the lines like what I’ve done for you :

9 101 solidworks 3dsketch tutorial

You have dimensioned all the lines but the sketch still not fully defined ( the blue lines) .

So what is the problem?!

The answer is 3d relations . as long as you drawing horizontal or vertical lines there will be no problem like this and dimensioning would be fine but we have a diagonal line here in the middle and the software need third dimension’s relation for this one . go to top view , this way you can understand what is going on , left click and hold the orange point shown below then move it up or down , release the mouse , system warns you that new relations will over define the sketch , click ok .

10 101 solidworks 3dsketch tutorial

See?! The diagonal line is not defined in the z direction . in order to fix the situation add a vertical relation between the diagonal line and the first line that you drew .

11 101 solidworks 3dsketch tutorial

In this step just fillet the corners to make a smooth profile .

12 101 solidworks 3dsketch tutorial 13 101 solidworks 3dsketch tutorial

Exit the 3d sketch .open a 2d sketch on front plane and draw circle like this :

14 101 solidworks 3dsketch tutorial 15 101 solidworks 3dsketch tutorial

Now we are going to create the first part of the frame . exit the sketch and on the features tab click swept boss/base . select the profile and path just like below :

16 101 solidworks 3dsketch tutorial 17 101 solidworks 3dsketch tutorial

In order to create another half of the frame we use mirror (mirror button is in features tab too) :

18 101 solidworks 3dsketch tutorial 19 101 solidworks 3dsketch tutorial

so far we have created the main body of the frame :

20 101 solidworks 3dsketch tutorial

 

Define a plane parallel to the right plane :

21 101 solidworks 3dsketch tutorial 22 101 solidworks 3dsketch tutorial

Click ok and open a 2d sketch on the new plane and draw just like the following picture .

23 101 solidworks 3dsketch tutorial

This is the path for next sweep so we need a profile too . open a sketch on front plane and draw a circle centered at the previous sketch . hide the plane1 .

24 101 solidworks 3dsketch tutorial

Sweep this circle along the path .

24 101 solidworks 3dsketch tutorial 25 101 solidworks 3dsketch tutorial

Now mirror the sweep2 by front plane . your part should looks like this :

27 101 solidworks 3dsketch tutorial

All that left to do is another support in width . we’ll create it now and then we will pattern it along the length of the frame . open another 3dsketch . click line and click on the origin draw a line along Y axis click and draw another line along X axis . then dimension the lines like this:

28 101 solidworks 3dsketch tutorial 29 101 solidworks 3dsketch tutorial

Now create the profile for this path . sketch a circle centered at the path in top plane :

30 101 solidworks 3dsketch tutorial

Sweep the circle along the path :

31 101 solidworks 3dsketch tutorial 32 101 solidworks 3dsketch tutorial

Click ok. Now we have this and all we have to do is to pattern the last sweep to complete the part

33 101 solidworks 3dsketch tutorial

Click on the linear pattern in features tab . you must select first direction now but there Is no edge on the part to be selected as direction . so what should we do now?! These profiles are circular so they have axis and we can use them as direction . in order to select an axis it must be visible to you , so go to view menu and select” temporary axis” . select the axis shown below and set the settings . if you can’t get the desired result just click on the “reverse direction” button :

34 101 solidworks 3dsketch tutorial 35 101 solidworks 3dsketch tutorial

Click ok to get the final shape and that’s it:

36 101 solidworks 3dsketch tutorial

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