Defining Dimensions in xDesign
As we’ve seen, one way to define the size and relationships between sketch objects is through constraints, which allows them to be adjusted in specific ways, depending on how the geometry is updated.
Adding dimensions is the other method for defining the size and relationships between sketch objects. Dimensions allow you to specify the exact size of the sketch elements by adding dimensions for linear distances, angles between lines, sizes of radii, and diameters of circles. Let’s examine how each of these can be added to this sketch to fully define the sketch.
To enable the “Dimension” command, simply click on the button in the action bar. With the button active, the cursor updates to show the dimension icon, and we can begin selecting sketch entities.
The first type of dimension that we want to add is the linear distance dimension. There are a few ways that a linear distance dimension can be created. The most common way is to simply click on a single line and click to place that dimension in free space. You then type in the dimension value, which we’ll set as 150 millimeters. Now the entire height of this line is defined in space. We’ll do this again for the bottom line, which we’ll set to 180 millimeters. And we’ll set the other edge to be 25 millimeters tall.
Another way to set a linear dimension is to select two lines that are parallel to one another. This will set the distance between them. For example, if we want to set the distance between the bottom edge and the horizontal line just above the arc, we can select the bottom edge and then click on the line right after, which allows us to set the distance between them, in this case we well set the distance as 60 millimeters. We’ll also set the distance between the edge on the left and the vertical line just above the arc. We’ll click the left edge, and then the other vertical line, and set the distance to be 105 millimeters.
Another way is to set a linear dimension is to select a line and a point. For example, we want to set the distance between this left edge and the point at the bottom of the angled line, which will determine the diameter at the base of the angled face of the “Revolve” feature. To do this, we’ll click the line on the left and the point at the bottom of the angled line, and set the distance to be 70 millimeters.
The last way to create a linear distance dimension is to select two points. This scenario can come up whenever a dimension needs to be set between two points that aren’t connected by horizontal or vertical lines. For example, let’s say we want to set a dimension between the upper left corner and the center point of the arc. We’ll click the first point and the second point, and then we can set the dimension in a few different ways. We can set the horizontal distance between them, the vertical distance between them, or the direct distance between the two points. In this case, we’ll set the direct distance between the two points.
This distance, however, was just a way to show you the options when dimensioning between two points, so we’ll click “Undo” to remove it.
The next type of dimensioning is creating an angle dimension. Creating an angle dimension can be as simple as selecting two lines that aren’t parallel to one another. In this case, we want to set the angle of the slanted line on the right relative to the vertical edge on the left. All you do is click on both lines, and then click to place the angle dimension. In this case, we’ll use an angle of 15 degrees. If you ever select two lines in xDesign thinking they’re parallel, and an angle dimension appears, this is an indicator that the lines aren’t actually parallel. Angle dimensions always appear when lines aren’t constrained to be horizontal, vertical, or parallel.
The next dimension type that we’ll examine is adding a radius dimension, which is applied to arcs and fillets in a sketch. This sketch has only one arc included, which we’ll dimension simply by clicking on it, and then clicking to set the radius value. We’ll set the radius to 15 millimeters. Notice that the dimension has the letter “R” in front of it, indicating that this dimension is setting the radius value of this sketch entity.
Notice that all the sketch entities have changed to black, which indicates that the sketch has gone from under-defined to fully-defined. This means that the sizes and relationships of all the sketch entities are set in place. They were also all created using the same “Dimension” command. However, let’s add one more sketch entity to learn how to add a diameter dimension. We’ll quickly draw a circle at the midpoint of the horizontal line shown below. This circle is now the only blue sketch entity showing it is the only under-defined entity. We’ll click the “Dimension” command, and then click on the edge of the circle to set the diameter. We’ll give it a value of 15 millimeters. Notice the diameter icon in front of the numerical value, which indicates that this is specifically a diameter dimension.
Now that we’ve covered the main dimension types added to this sketch, let’s look at another dimension type that can be helpful to include. “Driven Dimensions” are dimensions that don’t actually establish the size and relationships of sketch entities, but are “driven” by other dimensions and show a reference value on screen. For example, let’s say that we want to know the total height of the angled line. We can click on the top edge, click on the point at the bottom of the angled line, and place the dimension. This “driven dimension” appears in gray instead of black, making it easy to differentiate. We also can’t set a value since the dimension is determined by the other parts of the geometry, showing as 90 millimeters.
To set the total length of the angled line, we’ll click on the angled line shown here, which will create another “driven dimension”. At first, the same 90 millimeter dimension appears, but if we move the mouse upward, the dimension shifts to be along the angle of the line, indicating it’s total length.
To wrap up, let’s consider how to edit and delete dimensions. To edit a dimension value, simply double click on the numerical value. We’ll change this 150 millimeter dimension to 175 millimeters.
All the other black driving dimensions are maintained, however the values of the driven dimensions update to the new values. Let’s now delete the angled driven dimension. To delete a dimension, single click on the leader line of the dimension, and then press the “Delete” key, or click on the “Trash” icon on the context “toolbar”. This can be done for any dimension type.
Did you enjoy this series? Be sure to check back on the SOLIDWORKS Tech Blog to learn more about xDesign! Incase you missed it, take a look back on Part 1, Part 2 and Part 3 of the xDesign Sketching Series.