Insert a Company Logo Into a Drawing – SolidWorks Tutorial

A lot of companies like to have the company logo on their blueprints. The first step is to prepare your company logo. SolidWorks allows you to insert the following image types into a drawing: .bmp, .gif, .jpg, .jpeg, .tif, .wmf, .png, and .psd. Once your logo is ready to go, all you have to do is use the Sketch Picture command on the “Sketch” toolbar to easily insert your image file into a drawing.

To do this, open the drawing that you want to insert your picture in.

Then, pull down the “Insert” menu and pick Picture, or pick Sketch Picture from the “Sketch” toolbar.

In the Open dialog box, browse to an image file, then click Open.

Note that the inserted image is inserted in the lower left corner of the drawing, the (0,0) position. You can just drag and resize the images in the graphics area to any desired location.

In the Sketch Picture PropertyManager, pick the position, size, rotation, and transparency settings of your choice, and then, click the green OK check mark.

Sketch Picture PropertyManager

Just double click the image to open the Sketch Picture PropertyManager to make any changes. That’s it!

If you want your company logo in the background of every drawing, you can insert the picture while in Edit Sheet Format mode and save it as a Drawing Template.

Custom Wheel – SolidWorks Tutorial

This is a simple wheel design to shown you how it’s done. The main thing that you want to do is to get the main concepts for each step: the revolves, cut extrude at a specified direction, circular patterns, and cut revolve. Then, explore and create your own profiles to create your own wheels. If you are really proud of your work, I would love to see it. Just email me at info@AboutSolidWorks.com.

To start out, open a new part document. I used mm for my units. Start a sketch on the Front plane and draw the following sketch. The best way is to draw the basic shapes without the fillets and dimension it. Create about a 35mm vertical Line directly below the Origin and going downward. Continue with a second line about 9mm at 135 degrees, down and to the right. The third line continues down about 116mm, but at a sharper angle, just don’t let it lock in as vertical. Next, about a 62 mm line to the left and make it perpendicular to the third line. Then make about a 69 mm horizontal line to the right. The next line goes up about 32mm and to the right at about 60 degrees. And another one up and to the left about 120mm. This line will be parallel to the similar line shown to the left of it in the sketch (the third line). Now up about 13mm and to the left again, this one is at 135 degrees and is parallel to the second line. From here, create a vertical line which ends a little higher than the first one started but below the Origin. Then, finally close the loop.

Create one more line, a horizontal Centerline through the Origin. Then, add the dimensions below.

Then, add your fillets. Break the sharp corners with a 6 radius fillet. I did this in five places. I also turned off the sketch relations so that you could see the sketch better. (Pull down the “View” menu and uncheck Sketch Relations). Exit the sketch.

With the sketch selected in the FeatureManager design tree, click the Revolved Boss/Base button from the Features CommandManager tab, or pull down the “Insert” menu and pick Boss/Base – Revolve.

In the graphics area, pick the centerline of the sketch that goes through the origin. In the Revolve PropertyManager, make sure that the Angle is set to 360 and click OK.

That’s the first step to creating the wheel. Next, you are going to prepare for your cut that will reveal the spokes. To do this, create a new sketch on the Front plane, and sketch the two centerlines as shown below. Make sure that the angled centerline in coincident to the front edge line as shown by the black endpoint.

Exit the sketch. Now you are going to create a new plane by copying the Right plane at the endpoint of your angled centerline. To do this, in the FeatureManager design tree, click on Right Plane so that it is shown in the graphics area. Then, hold down the Ctrl key and drag the plane in the graphics area to the right and let go of the mouse button. In the graphics area, pick the endpoint of the angled centerline as shown below. Once the preview is correct, click OK in the Plane PropertyManager.

Start a sketch on the new plane that you just created. Pick the the outside circle and click Convert Entities from the “Sketch” toolbar in the CommandManager, or pull down the “Tools” menu and pick Sketch Tools – Convert Entities. Then create a small circle at the lower endpoint of the angled centerline from the previous sketch. Add two tangent angled lines, and then trim everything up as shown below. Right click on the top arc and pick Select Midpoint from the menu. Hold down the Ctrl key and pick the centerpoint of the small arc. In the Properties PropertyManager, pick the Vertical relation and click OK. Finally, add the two dimensions shown and exit the sketch.

With the sketch selected in the FeatureManager design tree, click the Extruded Cut button from the Features CommandManager tab, or pull down the “Insert” menu and pick Cut – Extrude.

In the Extrude PropertyManager, set the End Condition to Through All. Click in the Direction of Extrusion box. Then, pick the angled centerline from the graphics area, and then click OK.

Start a sketch on the Front plane and draw the sketch below. Make sure that the left most vertical line is Coincident to the Origin and the rightmost vertical line is Collinear to the right edge of the part, as shown below. Exit the sketch.

With the sketch selected in the FeatureManager design tree, click the Revolved Cut button from the Features CommandManager tab, or pull down the “Insert” menu and pick Cut – Revolve.

In the Cut-Revolve PropertyManager, click in the Axis of Revolution box. Then, pick the bottom horizontal line in the sketch. Make sure the Angle is set to 360 and then click OK.

Now, in the next step, you will create a circular pattern to create the rest of the spoke and lug nut holes. All you have to do is click the Circular Pattern button from the Features CommandManager tab, or pull down the “Insert” menu and pick Pattern – Circular.

In the CirPattern PropertyManager, click in the Features to Pattern box and then, in the flyout design tree, pick the Extrude and the Cut-Revolve. In the graphics area, pick the centerline of the part.  Make sure that the Angle is set to 360 and set the Number of Instances to ‘5‘. Click OK.

This is where you can play with the number of spokes by changing the Number of InstancesEqual spacing is easier to do than trying to calculate the angles manually.

Lastly, start a sketch on the Front plane and draw the following sketch. Make sure that the right side is Collinear to Plane1 and the top line of the sketch is Collinear to the bottom edge of the part.

Then, add your fillets. Start with the largest fillets first and work your way down. I also turned off the sketch relations so that you could see the sketch better. (Pull down the “View” menu and uncheck Sketch Relations). Exit the sketch.

With the sketch selected in the FeatureManager design tree, click the Revolved Boss/Base button from the Features CommandManager tab, or pull down the “Insert” menu and pick Boss/Base – Revolve.

In the graphics area, pick the horizontal centerline of the sketch that goes through the origin. In the Revolve PropertyManager, make sure that the Angle is set to 360 and click OK.

Modify Configurations – SolidWorks Tutorial

The Modify Configurations dialog box in SolidWorks 2008 makes it really easy to create and modify configurations for your parts and assemblies. In a part document file, configuring the dimensions and suppression states of your features and sketches got a lot easier to manage. Similar to a design table, all the parameters that you want to control are all in one place. And not just for one configuration at a time, but for all of your configurations.

Let’s take a closer look at the Modify Configurations dialog box. In a new Part document, create an extruded box with a length of 100, a width 50, and a height of 25, as shown below.

Right click on the 100 dimension and pick Configure dimension. Then, in the graphics area, double click the 50 dimension, and then, double click the 25 dimension. The dimensions should appear in the Modify Configurations dialog box when you double click on them.

The next step is to create the configurations that you want with the dimensions taht you want. It is pretty self-explanatory. In the Modify Configurations dialog box, right click on Default and pick Rename Configuration. Type ‘Medium‘ as the new name and click OK in the Rename configuration dialog box. Next, click in the < Create a new configuration. > cell and type ‘Large‘. Press the Enter key to accept the name.

Click in the < Create a new configuration. > cell and type ‘Small‘ to create a third configuration. Press the Enter key to accept the name. Now, all that’s left is to change the numbers. Note that you can resize the Modify Configurations dialog box by dragging the edges to whatever size that you like.

Once your dimensions are set the way that you want them, click OK. If you are asked to rebuild your model, click Yes. In the Design tree area, click on the ConfigurationManager tab and you will see your new configurations.

Double click the different configurations and watch your part change size. Note that you can change the active configuration while you are in the Modify Configurations dialog box as well.


In an assembly, you can use the Modify Configurations dialog box to configure configurations of components suppression states, and dimensions of assembly features and mates.

That’s it!