SolidWorks 2010
Chapter 4–Introduction to Extruded Parts
In this lesson we will create extruded sections and create extruded cuts.
Please note. Read the text of the notes carefully, the pictures are only there as a visual check.
Before creating any 3D model or 2D drawing, consider the term “Design Intent”. Think about which plane you want to draw the part on, adding cuts and other features and how it would be easiest to reference and constrain them.
Create a new part as described on page 19 of chapter 3.
First we are going to create a simple rectangular extruded block. Then we will cut some holes in it and add some extruded features to it.
From the top left corner, select the Extruded Boss/Base icon, as shown below.
Each of the 3 available planes should now be highlighted in the drawing area, as shown below.
Any of these planes may be selected, but, for the purpose of this exercise, move the cursor to the top corner of the Right Plane, as shown below. The plane will be highlighted and to select it click the left mouse button.
The view will rotate around until you are looking directly at the selected plane, as shown below.
Once rotated the plane will disappear leaving you with just the origin point (shown in red in the centre of the screen), as shown below.
To draw a rectangle the simplest way is to use the Corner Rectangle tool. To select this pick the pull down menu at the side of the rectangle tool (circled in red) and select the Corner Rectangle, as shown below.
Now as you move the cursor over the origin point you should see a red dot appear, as shown below.
When the red dot is visible, click the left mouse button once and release it. This selects the starting corner of the rectangle. As you move the mouse you’ll see that the opposite corner of the rectangle moves according to the position of the mouse, a bit like it’s attached via an elastic band, as shown below.
The other fact that you should notice is the size of the rectangle given as x and y co-ordinates. This allows you to make the rectangle approximately the correct size that you require.
In this case we require a rectangle x100 y50, so move the corner of the rectangle to approximately the correct position and click the left mouse button again to select its position, as shown below.
Once you select the second corner of the rectangle, you will be left with a green rectangle, as shown below.
Now move the cursor away from the rectangle a little and click again. You will have a rectangle with 2 black lines and 2 blue lines, as shown below.
The black lines mean that they are constrained, in this case fixed to the origin point. The blue lines however are now constrained and if you select one of these, click the mouse and hold the button down, you’ll see that the line can be moved and its adjoining lines stretched as you wish. This is not good, as the rectangle could become any size, rather than being fixed to the exact size that we require.
The way that we constrain, or fix the size of a part is by dimensioning it. To do this select the Smart Dimension icon from the top of the screen, as shown below.
There are 2 ways to dimension any given line. The first is to select the line itself by selecting the line anywhere along its length. The second is to select the two end points of the line. Either way will result in a dimension appearing which you can position in an appropriate place, as shown below.
Once you click to drop the dimension, a menu will appear allowing you to edit that dimension to the required value, as shown below.
In this case as we require a rectangle which is 100mm x 50mm, we simply type in 100 (as circled in red), then click the green tick (as circled in green), as shown below.
You will notice that one of the lines which was blue is now black, that is because the length is now constrained, as shown below.
Now repeat this process for the vertical line and set it to 50, as shown below.
The sketch of the rectangle is now complete and constrained. You can now leave the sketch stage by clicking the end sketch icon in the top right corner (as circled in red), as shown below.
The extrude menu will now appear asking you how thick(D1) you wish the extrusion to be (as circled in red), as shown below.
This menu also allows you to select the direction of the extrude (circled in red) or the option of extruding the part either side of the plane you have been drawing on, or mid plane (circled in green), as shown below.
For the purposes of this exercise, we will select the thickness as 20 (circled in red) and leave the other settings as the default. Once this has been completed, click the green tick (circled in black) as shown below.
You now have a 3 dimensional block, 100mm long x 50mm high x 20mm thick, as shown below.
To rotate the block around to view it 3 dimensionally, press down and hold the centre mouse button and as you move it, you will notice the block rotates.
To bring the block back to an isometric view point, from the View Orientation menu at the top of the screen, select the Isometric icon and click once. Alternatively, hold down the Ctrl button and press the number 7 on the keyboard, as shown below.
Your block should now be positioned as shown below.
Drawing a shape to form an extruded feature is not just confined to sketching on a plane, you can also pick any face of a 3D model to sketch on. In the following exercises on extruding and creating an extruded cut we will review the principles and steps required.
As before, click on the Extruded Boss/Base icon and this time select the largest front face of the block, as shown below.
Unlike the last time, the view will not automatically rotate to allow you to look straight at it. This time you need to rotate it manually. You do this by opening the View Orientation menu and clicking on the icon named Normal To, as shown below.
Your model view will then rotate so that you are looking straight at the face you have selected, as shown below.
While this step is not essential, it certainly makes drawing, dimensioning and therefore constraining much simpler.
Next we are going to create a 20 x 20 square section extruding from the lower left corner.
So using either the rectangle tool, or the line tool, drawer the square and constrain it by dimensioning (so that all the lines are black), as shown below.
As before, once you have completed the sketch, click on the end sketch icon in the top right corner, as shown below.
At this stage you may wish to rotate the model to ensure that the extruded feature is projected in the right direction. Make this feature 30mm long and click the green tick once complete. You model should now look like the one shown below.
The final exercise for this block is to create a circular cut through the 20 x 20 square extrusion.
To do this, select the Extruded Cut icon, as shown below.
Now select the face of the 20 x 20 square extrusion, as shown below.
As before, using the View Orientation menu, rotate your model so that this face is Normal To where you are looking from, as shown below.
To draw a circle to produce a circular cut, click on the Circle icon (circled in red), as shown below.
Now drawer and dimension the size and position of the circle as shown below. When dimensioning circles, if you click anywhere on the circumference, the dimension will automatically be generated from the centre point.
As before, once you have completed the sketch, click on the end sketch icon in the top right corner of the screen and rotate the view to allow you to see where the cut is going, as shown below.
As you can see from the picture above, the length of the cut has defaulted to the last input 3D dimension which was 30mm. This cut length maybe altered to suit. Alternatively, the Direction 1 menu has many other options, as shown below.
For this exercise, select the Through All option and click the green tick to accept.
Your model should now look like the one in the picture below.
We are going to add one final cut feature to this model, a hexagonal hole 10mm deep on the large front face.
Just as you have done before, select the Extruded Cut icon and click on the large front face of the model, the same one you selected when drawing the 20 x 20 square. Rotate the view of the model so that this face is Normal To your viewpoint.
Now select the Polygon icon, as shown below.
There are various options available on the Polygon menu, as shown below. The only one that we are interested in at this stage is that the number of sides option is set at 6 (circled in red).
Now click on the lower right corner of the face to select a position for the centre point of the hexagon. Then moving the cursor away from the centre, select a suitable place to click to determine the size and orientation of the hexagon, as shown below.
To constrain the hexagon we need to input the following information:
- The position of the centre of the hexagon, both in the x and y planes
- The size of the hexagon, generally measured between the two opposing faces
- The angle of the hexagon in relation to a fixed edge of the block.
So dimension the hexagon as shown below.
Unlike the circle drawn previously, if you want to dimension the centre point of the rectangle, you must select the centre point, not the edge.
As before, once you have completed the sketch, click on the end sketch icon in the top right corner of the screen and rotate the view to allow you to see where the cut is going. Make the depth of this cut 10mm, as shown below.
Exercise complete, don’t forget to save this part, we will be using it again later.
Now create extruded 3D models of the parts shown below.
CAD – Chapter 4 - Paul Mulder
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