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
or read the tutorial here:
we will create this frame during the 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
- Smart dimension
- Swept boss/base
- 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
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 .
Don’t exit the line . press tab once to switch to XZ plane and draw a line in x direction .
Press tab and sketch along Y and click again .
Exit the line . now your sketch must be like this :
Select the line again and click on the last point. Sketch a line like this in the XY plane .
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 :
Now dimension the lines like what I’ve done for you :
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 .
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 .
In this step just fillet the corners to make a smooth profile .
Exit the 3d sketch .open a 2d sketch on front plane and draw circle like this :
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 :
In order to create another half of the frame we use mirror (mirror button is in features tab too) :
so far we have created the main body of the frame :
Define a plane parallel to the right plane :
Click ok and open a 2d sketch on the new plane and draw just like the following picture .
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 .
Sweep this circle along the path .
Now mirror the sweep2 by front plane . your part should looks like this :
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:
Now create the profile for this path . sketch a circle centered at the path in top plane :
Sweep the circle along the path :
Click ok. Now we have this and all we have to do is to pattern the last sweep to complete the part
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 :
Click ok to get the final shape and that’s it: