SolidWorks 2011 Parts Bible - Matt Lombard [46]
The Circle tool creates a circle using one of two methods, which are available from either the flyout icon or the Circle PropertyManager:
• Center Creation. Click the center of the circle and drag the radius. The Circle PropertyManager calls this function center creation.
• Perimeter Creation. To create a circle using this technique, you must select the Perimeter Creation option from the Circle PropertyManager window after clicking the Circle tool. There is also a separate Perimeter Creation toolbar button and a menu selection for Tools⇒Sketch Entities⇒Perimeter Circle. This only creates tangent relations with other entities in the current sketch; if you are building a circle from model edges or entities in other sketches, you need to apply the relations manually. SolidWorks calls these functions perimeter creation.
• Tangent to Two Entities. Start the circle with the cursor near one line in the sketch. A Tangent symbol appears by the cursor with a yellow background. Click and drag the diameter to the second tangent entity, where a similar cursor symbol should appear. Release the mouse button and right-click the green check mark icon. This process is shown in Figure 3.6.
Figure 3.6
Creating a perimeter creation circle
• Tangent to Three Entities. Use the same process for Tangent to two entities, but omit the right-click of the green check mark icon. After dropping on the second tangent, drag again to the third tangent entity.
The Centerpoint Arc tool creates an arc by clicking the center, dragging the radius, and then clicking and dragging the included angle of the arc. The first two steps are exactly like the Center-Radius circle.
The Tangent Arc tool creates an arc tangent to an existing sketch entity. Depending on how you move the cursor away from the end of the existing sketch entity, the arc can be tangent, reverse tangent, or perpendicular, as shown in Figure 3.7.
FIGURE 3.7
Using the Tangent Arc feature
Another way to create a tangent arc (called auto-transitioning) is to start drawing a line from the end of another sketch entity, and while holding the left mouse button, press the A key; or return the cursor to the starting point and drag it out again. This second method can be difficult to master, but it saves time compared to any of the techniques for switching sketch tools.
The 3 Point Arc tool creates an arc by first establishing endpoints, and then establishing the included arc, as shown in Figure 3.8. Again, this tool also works using the click+click or click and drag methods.
FIGURE 3.8
Creating a three-point arc
The Sketch Fillet tool creates a sketch fillet in one of two ways. Either you can select the endpoint where the sketch entities intersect or you can select the entities themselves, selecting the portion of the entity that you want to keep. Figure 3.9 illustrates both techniques.
FIGURE 3.9
Creating a sketch fillet
The Sketch Chamfer tool is on the same flyout as the Sketch Fillet by default. Sketch Chamfer does not have a list selection box the way that fillet does, and does not use a preview like the fillet.
Sketch Fillets
While the Sketch Fillet tool is easy to use and may align with your way of working in a 2D program, it is not considered best practice to use sketch fillets extensively. Some reasons for this include:
• Large changes in the size or shape of the rest of the sketch can make the feature built from the sketch to fail.
• SolidWorks (and other parametric programs as well) often has difficulty solving tangent arcs in some situations. You may see fillets flip tangency or go around 270° instead of just 90°. Using many fillets in a sketch can often cause trouble.
• If you want to remove the fillets temporarily, there is no good way to do this if you have used sketch fillets.
• Sometimes feature order requires that other features,