Tinndahl’s Tip from The Train: Sketches and Features

When working in SOLIDWORKS (or any CAD program for that matter), it is better to work smarter not harder.

In my previous article, Tinndahl’s Tips for SOLIDWORKS Customization, I went through how you can customize your user experience. In this and the next article, I am going to look into some tips and tricks of the usage of SOLIDWORKS.

Before the First Sketch

There are a few settings I want to ensure are present before I start on a sketch. These settings are done within the system options, so you do not need to do this every time.

Please note that these are my preferences and, as with all customizations, you might find that you do not agree with them. Feel free to customize my customizations and make them your own.

Sketch Options

Let’s start with the sketch options listed in the System Options.

In this pane there is one checkmark that I always make sure is set, and a few optional checkmarks.

I always want a checkmark in “Auto-rotate view normal sketch plane on sketch creation and sketch edit” (1) as this will ensure that my view rotates to be directly in front of me when I create a new sketch or edit an existing sketch.

Next, you might want to consider checking off “enable on screen numeric input on entry creation” (2), as this allows you to create dimensions automatically when you do a sketch.

As a rule of thumb, I also set a checkmark in “Create Dimension only when a value is entered” (3). With this set, I can decide when I want to add a dimension.

The final checkmark is only a recommended setting—not a required one—if you are in the habit of not fully defining your sketches. I follow the “fully define every time” rule.

The checkmark I am referring to is “Always use fully defined sketches” (4) which will make sure that you cannot exit a sketch unless it is fully defined (all black).

Selecting with Care

While SOLIDOWORKS has a wide range of selection tools, I will just touch on two different methods: Lasso Selection and Box Selection.

To activate these selection tools, right click on your work screen and select “Selection tool,” then select your weapon of choice.

The lasso tool gives you the option to create an organically-shaped selection field, while the Box Selection provides only a rectangle-shaped field.

With either one, you will notice a color overlay that shows where the selection is made. And you will also notice that the color differs depending on which way you move your mouse. Move the mouse from right to left and the color is green. Move from the left to right, and the color is blue.

The blue color (left to right) indicates that only sketch segments completely within the selection box will be selected.

When green (right to left), anything that the selection field touches and is inside the selection field is selected.

Shortcuts to Success

SOLIDWORKS has a wide range of predefined shortcuts, which you might find useful.

These shortcuts can be changed (for more information on that, see my previous article), but for now I will give you my favorite default shortcuts.

After starting a sketch, you can use the “L” key to start a line. Whenever you start any sketch, you can see a number of options in the left-hand side of the screen. If you hold down the “ALT” button on your keyboard, you will notice that one letter in each command is underlined.

If you continue to hold down “ALT” and press one of these letters, the corresponding command will be activated for this sketch segment. For instance, “ALT” plus “C” will ensure that the sketch segment is created as a construction line.

The commands may differ in the different sketch segments; for instance, a circle does not have the horizontal option.

Some of these commands are also available after the sketch has been created. All you need to do is select one or more segments.

Of course, SOLIDWORKS has commands in the toolbar to move or copy your sketch segments, but there are also shortcuts that can help you with this.

By selecting one or more sketch segments and holding down “SHIFT” you can move your sketch. However, keep in mind that all relations still apply: If a sketch point is anchored to one point, it will stay anchored and your sketch will change according to the new circumstances.

If you hold down “CTRL” while dragging the selected sketch segments, the selection will be copied to the new location.

The “Power trim” tool is very popular. While selected, can you quickly trim your line to the closest sketch segment. However, by selecting the power trim and holding down the SHIFT key, the tool becomes the “Power extend,” which extends the line to the nearest line.

What’s in the Box

For this article, I will create a visual, not functional, representation of a chess clock.

As I want to be able to control my box with equations, I start off by opening the equation dialog box by right clicking on it in the feature tree and choosing “manage equations.” Or, go to Tools > Equations.

I start off by creating three global variables called “Length,” “Height” and “Depth” and assigning values.

By using variables, I can easily change the size of the model.

Within my sketch, I create a rectangular segment and set the length to the “Length” equation by starting with an equal sign (=).

This allows me to select between global variables, properties and a set of predefined functions.

The other dimension is given the height value, and the box is dimensioned.

For reasons that will be revealed later, I am going to make sure that the center of the box is in the origin of the model. This also means that I want to extrude it by the same amount in each direction.

Normally this would require that I use the Midplane Extrude. However, I want to use the thin feature and create a hollow enclosed box.

If I select the midplane, it is not possible to select the “cap” ends which would close off the box.

Instead, I am going to extrude it into each direction.

In the value field, I am going to add “=” and select the depth equation, and add a “/2” to divide by 2.

Before pressing “OK” ensure that there is a checkmark in thin feature and endcaps Again, I add the “=” and the right thickness.

In the equation list, the new equations have been added under “equations.”

For this next part I want to create two holes for the switches and two holes for the clock faces.

To start, I create a sketch on the top plane (located in the middle of the model) and create a line that is coincident on both sides of the model, placing it 60 mm from the front edge of the box.

The line is now fully defined (notice the relations and the one dimension).

This line will be used as the base for my holes in both the top of the box (the switches) and the front of the clock (the clock face). But I want to make sure that I have reference points for these cutouts, which is why I am going to use the “Segment” feature.

With the sketch still active, I go to Tools > Sketch Tools > Segment.

This feature allows me to either split the line into multiple segments, or to insert a number of points with equal distance. In this case, I will insert three sketch points.

With this, I am ready to create the cutouts for my clockfaces.

Within a new sketch on the front of the clock, I create two circles and give one of them a radius of 100 mm. Then I select the center point, hold down CTRL key and select one of my sketch segments in the previous sketch and select “coincident.”

I have to do the same with the other circle. Finally, I create an equal relation between the two circles.

Next, I create an “Extrude Cut,” and ensure it is up to next, in case I want to change the thickness later.

Since I know I am going to change the shape of the top of the clock in the next article, I will do the holes for the switch on the top plane.

This time, I only create one circle, attach it to the sketch segment as previous and give it a dimension. With the sketch still active, I create a mirror feature, select the circle to ensure that there is a checkmark in “Copy” and in “Mirror about,” then select the right plane.

This creates a mirrored version of the circular sketch that updates with the original sketch.

Afterwards, I create an extrude cut and with added material the box for my clock is ready.

In the next article, I will be modifying the top of the clock, adding fillets and a bottom, and creating an assembly with clock hands that move according to each other.

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