Little shortcuts in sketching can add up to big savings over the course of a modeling session.
Part modeling in SOLIDWORKS is the meat and potatoes, the block and tackle, the big fish to fry … let’s just say it’s fundamental to using SOLIDWORKS.
Part modeling begins with sketching. It’s the first lesson for beginners learning SOLIDWORKS, but it’s also the first place I point experts to who are looking to improve their overall skills and get faster with using SOLIDWORKS. In this article, I’ll share with you my favorite tools and tips to help beginners and experts alike who want to improve their skills and get some time back in their day by sketching faster.
Relations—Adding from Shared Vertex (Introduced in 2015)
Tip: Save time and clicks. Instead of selecting multiple sketch entities to add a relation, pick the shared point between entities to add a relation.
Adding sketch relations like perpendicular or tangent between two line segments is pretty straightforward. Prior to 2015, this had to be done by holding the control key and selecting both lines, but this took two clicks. Now you can save a step by adding a relationship to a vertex with one click. If there are line segments (circular or linear) adjacent to the vertex, then the appropriate relation can be added, saving you clicks and time. These clicks add up to make a big difference. Like the difference between meeting a deadline or passing the Certified SOLIDWORKS Professional (CSWP) exam.
Angle Dimensions with the “Biad” (Introduced in 2015)
Tip: Save time and clicks. Leverage this functionality to define angle dimensions without adding extra construction geometry.
When you want to add angle dimensions to a line, you have to reference something. This is typically some other existing geometry, or you can add construction geometry whose sole purpose is to exist as an angle reference. But it doesn’t have to be this way if you know the special click sequence that will activate the “biad.” The biad is like the triad but for two dimensions. It was introduced in 2015 and offers a way for you to leverage a virtual construction line at a line’s endpoint. The trick is the click sequence. With the Smart Dimension tool, activate the biad with your first click on the line. Then click on its endpoint. Finally, you should click on the desired reference axis. That’s how you can save a lot of time and clicks when adding angle dimensions.
Horizontal or Vertical—How to Know What’s Up (Introduced in 2015)
Tip: Save time and headaches. Quickly identify the correct relationship so you don’t make a mistake and make the geometry go crazy.
SOLIDWORKS has three default planes—front, top and right. But the number of planes goes up quickly when you’re creating a lot of complex geometry. You can find yourself in some weird perspectives when creating geometry, so it helps to know which way is up. This helpful indicator acts as your North Star when you’re adding horizontal or vertical relations to lines. When you click on a line, whatever is the “closer” relation is the one that is either bold in the PropertyManager (on the left side) or highlighted in the context menu in the graphics area.
Power Trim, Power Extend, and Power Detach
Tip: Save time and clicks. The Power Trim tool is a workhorse for sketching. Learn all its functionality and you’ll be sure to agree.
If all you have is a hammer, everything looks like a nail. But if all you have is Power Trim, you have a weed whacker because it’s really capable. Click and hold, and any geometry you pass over will be whacked or trimmed away. If you make a mistake, that’s okay. Retrace your steps and pass over the red square to undo the last trim.
Power Trim goes beyond trimming. It can also extend. The trick is to click and hold while you’re on top of geometry. This is how you can add to or extend geometry. Lastly, you can detach sketch entities from each other by clicking first on a vertex and then dragging an entity off.
Power Trim is incredibly useful. If I had to take one SOLIDWORKS tool with me to a desert island, this would be it.
Think Outside the Box Selection (Introduced in 2014)
Tip: Save time and clicks. There are different selection tools you can use, and they behave differently depending on the direction you use them.
The default selection method is the box selection tool. As you draw a box to select folders or files in Windows Desktop, you can select SOLIDWORKS entities with a box. But did you know that this works two different ways depending on the direction? Look closely the next time you use it and you’ll notice even the color of the box is different depending on the direction—left to right is blue and right to left is green. Green means go, as in anything that the selection touches will be selected. Blue (left to right), however, has to be completely within the selection to be selected.
But don’t get boxed in. You can also switch the selection tool to the lasso. This offers more control over your selections. Just like with the box selection, the functionality depends on the direction.
Invert Selection—Picking This or That
Tip: Save time and clicks. Pick something, then pick its opposite!
The best way to do something in SOLIDWORKS is the quickest way. When it comes to selection, there are two ways to do it. You can either select what you want, or you can select what you don’t want and then invert the selection to give you what you want.
Intersections and Virtual Sharps
Tip: Save time and headaches. You can add geometry at the virtual intersection of any two nonparallel lines.
Virtual sharps are the virtual points at the intersection of two lines. There are two ways you can add them and neither of them is straightforward or obvious. The most common way is to first select both entities and then click the sketch point to add a point at the intersection. The other way is to leverage the Smart Dimension functionality to directly add a virtual sharp while adding dimensions. This is great because more often than not, you are creating a virtual sharp because you want to add a dimension. With the dimension tool active, just right-click on a line and then select the intersection command. You will then select the second line and you can add a virtual sharp from within the tool. This is the fastest way to add virtual sharps for dimensioning.
