## 3D Modelling in SolidWorks – By Samarth Mahajan

This tutorial is our own walk-through of the instructions given in this document
: http://www.scribd.com/doc/6793518/30-Minute-Lesson.  . We have taken screenshots at a number of steps which might (hopefully) give you a better idea of SolidWorks than the original document.

SolidWorks is a 3D mechanical CAD (computer-aided design) program. SolidWorks is currently used by over 1.3 million engineers and designers at more than 130,000 companies worldwide. Unlike max, this software is more professional in the sense that it is used mostly by professionals in the field of mechanical engineering to make parts and drawings for various components of a machine. Like the previous max series, the SolidWorks tutorial series is also divided into two parts. In the first part we will look into some general applications of an engineer’s modelling software like creating base, boss, and cut features, adding fillets and creating patterns. In the second part we will highlight some important tools in SolidWorks which can come in handy for engineering and design purposes and are generally not present in other modelling packages.
This tutorial includes the following parts:

### Creating a circular pattern

For your first part, you create the pressure plate shown below. A part is a 3D model made up of features.
You begin this exercise by creating a new part.
1. Click New  on the Standard toolbar.

The New SolidWorks Document dialog box appears.

1. Click Part.
2. Click OK.

A new part window appears.

### Sketching the circle

The first feature in the part is a cylinder extruded from a sketched circular profile.

1. Click Extruded Boss/Base on the Features toolbar.

The Front, Top, and Right planes appear in the graphics area.

1. Move the pointer over the Top plane to highlight it, then click to select it.

The display changes so that the Top plane is facing you. A sketch opens on the Top plane.

1. Click Circle on the Sketch toolbar.

The Circle PropertyManager opens in the left pane.

1. Move the pointer over the origin.

The pointer changes to. This indicates a coincident relation between the center of the circle and the origin.

1. Click to place the center point on the origin.
2. Move the mouse and notice a preview of the circle dynamically follows the pointer.
3. Release the mouse and click in the PropertyManager to finish the circle.

Now add a diameter dimension to the circle.
1. Click Smart Dimension on the Sketch toolbar.
2. Select the circle.

Notice the preview of the diameter dimension.

1. Move the pointer to where you want the dimension and click to add the dimension.
2. In the Modify box, type 128, then click and click in the graphics area.

### Extruding the Base Feature

Extrude the 2D sketch to create the 3D cylinder.
1. Click Sketch on the Sketch toolbar to exit the Sketch.

You exit the sketch when you are done with the 2D profile and are ready to create the 3D cylinder.

The settings for the extrusion appear in the PropertyManager in the left panel.

1. In the PropertyManager, under Direction 1:

1. Select Blind in End Condition.
2. Set Depth to 7.

Notice the shaded preview of the extrusion.

1. Click.

The first feature is complete. Extrude1 appears in the FeatureManager design tree in the left panel.

Saving the part
1. Click Save on the Standard toolbar.
2. In the dialog box, type Pressure_Plate for File name.
3. Click Save.

The extension .sldprt is added to the file name, and the file is saved.

### Sketching the boss

Create a sketch for the ring boss.
1. Click Extruded Boss/Base on the Features toolbar.
2. Select the top face of the part.
3. Click Top on the Standard Views toolbar.
4. Click Circle on the Sketch toolbar.
5. Move the pointer over the origin.

The pointer changes to.

6.   Click to place the center of the circle.

7.   Move the pointer to create the circle.

8.   Release the pointer and click in the PropertyManager to finish the circle.

### Dimensioning the boss sketch

1. Click Smart Dimension on the Dimensions/Relations toolbar.
2. Select the circle.
3. Move the pointer and click to place the dimension.
4. In the Modify box, type 75, then click and in click in the graphics area.

### Offsetting Entities

The sketched circle represents the outside of the ring. Next create the inside of the ring using the Offset Entities tool.
1. Click Offset Entitieson the Sketch toolbar.
2. In the PropertyManager, under Parameters:
1. Set Offset Distance to 5.
2. Select Reverse to offset the circle to the inside.
3. Select the sketched circle.

1. Click.

### Extruding the Ring Boss

Now that the sketch is complete, extrude the sketch to make the ring boss.
1. Click Sketch on the Sketch toolbar.
2. Click Trimetric on the Standard Views toolbar for a better view of the model.
3. In the PropertyManager, under Direction 1, set Depth to 12.
4. Click.

### Sketching the Hole

Create a circle for the center hole.
1. Click Extruded Cut on the Features toolbar.
2. Select the top face of the part.
3. Click Top on the Standard Views toolbar.
4. Click Circle on the Sketch toolbar.
5. Move the pointer over the origin.

The pointer changes to.

1. Click to place the center of the circle.
2. Move the pointer to create the circle.
3. Release the pointer and click in the PropertyManager to finish the circle.

### Dimensioning the Hole Sketch

1. Click Smart Dimension on the Dimensions/Relations toolbar.
2. Select the circle.
3. Move the pointer and click to place the dimension.
4. In the Modify box, type 25, then click and click in the graphics area.

### Creating a Hole

Cut a hole through the center of the part.
1. Click Sketch  (Sketch toolbar).
2. Click Trimetric  (Standard Views toolbar).
3. In the PropertyManager, under Direction 1, select Through All for End Condition.
4. Click.

Add a fillet feature to round off the edges of the part.
1. Click Fillet on the Features toolbar.
2. Click Trimetric on the Standard Views toolbar for a better view of the model.
3. In the PropertyManager, under Items To Fillet, set Radius to 2.
4. Select the top face of the ring boss and the outside face of the base.

1. Click

### Sketching the Tall Cylinder Extrusion

Sketch a circle for the tall cylinder extrusion.
1. Click Extruded Boss/Base on the Features toolbar.
2. Select the top face of the base cylinder.

1. Click Top on the Standard Views toolbar.
2. Click Centerline on the Sketch toolbar.
3. Move the pointer over the origin until the pointer changes to and click to start the centreline.
4. Move the mouse above the start of the centreline.

The pointer changes to to indicate the centreline is vertical.

1. Make the line about 45mm long.
2. Release the pointer and click twice to end the line.

### Sketching the Tall Cylinder Extrusion (continued)

1. Click Circle on the Sketch toolbar.
2. Move the pointer over the endpoint of the line (not the endpoint by the origin). The pointer changes to.

10.  Click to start the circle.

11.  Move the pointer to define the circle and click to finish.

### Dimensioning the Tall Cylinder Sketch

1. Click Smart Dimension on the Dimensions/Relations toolbar.
2. Select the circle.
3. Move the pointer and click to place the dimension.
4. In the Modify box, enter 27 for the circle dimension, click, and click in the graphics area.
5. Select the vertical centerline.
6. Move the pointer and click to place the dimension.
7. In the Modify box, type 35 to position the circle, click, and click in the graphics area.

### Add the Tall Cylinder Extrusion

Now that the sketch is done, make the extrusion for the tall cylinder boss.
1. Click Sketch on the Sketch toolbar.
2. In the PropertyManager, under Direction 1, set Depth to 30.
3. Select the circle to define the Selected Contours.

1. Click.
2. Click Trimetric on the Standard Views toolbar for a better view of the model.

### Sketching the Tall Cylinder Hole

Make a sketch for a hole through the tall cylinder extrusion.
1. Click Extruded Cut on the Features toolbar.
2. Select the top face of the tall cylinder extrusion.
3. Click Circle on the Sketch toolbar.
4. Move the pointer to the edge of the tall cylinder and leave it there until the center point of the tall cylinder appears as shown.

1. Move the pointer over the new center point.

1. Click to place the center of the circle.
2. Move the pointer and click to finish the circle.
3. Click.

### Dimensioning the Tall Cylinder Hole Sketch

Add a dimension to control the diameter of the circle.
1. Click Smart Dimension on the Dimensions/Relations toolbar.
2. Select the circle.
3. Move the pointer and click to place the dimension.
4. In the Modify box, type 15, click, and click in the graphics area.

### Adding the Tall Cylinder Hole

Create a hole in the tall cylinder that cuts through the entire part.
1. Click Sketch on the Sketch toolbar.
2. In the PropertyManager, under Direction 1, select Through All for End Condition.

1. Click.

### Adding Fillets to the Tall Cylinder

1. Click Hidden Lines Visible on the View toolbar.

This shows the edges needed for the fillet.

1. Click Fillet on the Features toolbar.

The radius is already set to 2mm to match the last fillet you added to the model.

1. Select four items for the fillet as shown:

• The top face of the tall cylinder extrusion.
• One edge on each side of the tall cylinder where it intersects the ring extrusion.
• The edge of the hole that cuts through the tall cylinder on the bottom of the first extrusion.

1. Click.
2. Click Shaded With Edges on the View toolbar.

### Creating a Circular Pattern

Create six tall cylinder extrusions with cuts and fillets evenly spaced about the central axis of the part using the Circular Pattern tool.
1. Click View, Temporary Axes.

This shows all of the system-generated axes in the part. You select one as the central axis of the pattern.

1. On the Features toolbar, expand the Linear Pattern flyout toolbar and click Circular Pattern.
2. In the PropertyManager, under Parameters:
1. Select the temporary axis in the center of the part for Pattern Axis.
2. Select Equal spacing to pattern the number of instances uniformly around the axis within 360°.
3. Set Number of Instances to 6.
3. Click in Features to Pattern.
4. In the flyout FeatureManager design tree in the graphics area, select the last three features (Fillet2, Extrude7 (the cut extrude), and Extrude6).

1. Click.

The last feature is a fillet that runs around the inside and outside edges of the patterned items.
1. Click View, Temporary Axes to turn off the system axes.
2. Click Fillet on the Features toolbar.
3. Select two edges as shown. You need to select one edge on the inside of the ring and one edge on the outside of the ring.

1. Click to add a 2mm fillet.
2. Click Save on the Standard toolbar.

The part is complete.

### Summary

By following this tutorial and experimenting with features similar to those mentioned in this exercise, you will be able to make most of the parts that are needed in a mechanical assembly. Be sure to explore other features too which were not touched while modelling this pressure plate.