Sketches are such an  important aspect of SolidWorks. Virtually everything that is modeled in SolidWorks is controlled by a sketch. Yet, It still amazes me how even though everybody creates sketches daily, a lot of users aren’t aware of all the cool sketch tools available. Over the next couple of weeks we will look at some the the lesser known sketch tools available that will ultimately help you creating better sketches.

Split Entities

How many times have you looked at a sketch segment and decided that it should be two segments? How many times have you trimmed the segment and created another segment separately? How many times? In the past I was guilty of this, that was until I discovered the Split Entities command. Look at the following sketch. Let us suppose that we need the arc and vertical line each split into two segments.

The quickest and easiest way to split these sketch entities is to use the Split Entities tool in Tools -> Sketch Tools.

When the Split Entities tools is activated the pointer will change. Select the location of the split point on the segment.

The segment will be split into two segments and a split point is added between the two segments.

Removing Split Points

If at anytime you decide that two separate segments, that were created using Split Entities, need to be joined again; the split point can be deleted. Click the split point…

…and press Delete on your keyboard. The split point will be removed and the single segment will be restored. NOTE: You can only delete points created using Split Entities. You cannot delete line and arc endpoints in this manner.

Splitting Circles, Ellipses and Closed Splines

In order to split a closed entity such as a Circle, Ellipse or closed Spline; two split points must be added.

With the Split Entities tool activated, select the first point on the circle.

Notice that a split point is not added, instead a point is added for reference for the time being. A second point on the circle must be selected before the split points are added.

After selecting two points, the circle is now split into two separate arcs.

Jog Line

Sketch lines can be jogged in 2D and 3D sketches. When using the Jog Line command, jog lines are automatically created with parallel and perpendicular constraints and can be dragged and dimensioned to size. To illustrate the Jog Line, we are going to add a jog to this single line.

Select Jog Line in Tools -> Sketch Tools.

Select the line for the first point of the jog and select the second point. It much like creating rectangle, dragging the second point around before clicking will give you a preview of the height and width of the jog. When you are satisfied with the jog click the mouse button.

The jog has been added to the line and all that is left to do is to dimension the jog. As I mentioned earlier, the parallel and perpendicular lines already have the appropriate relations added.

Create Sketch from Selections

Sometimes you want a new sketch to be based on other sketch elements. Using Create Sketch from Selections makes it so much easier to create a new sketch from a selection of sketch entities. In the past I have created a new empty sketch and used Convert Entities to trace segments from another sketch, it works but it does require extra steps such as showing and hiding sketches. It is so much easier when using Create Sketch from Selections. Say for instance, we want a new sketch with only the the larger circle and key way from the sketch below.

In the sketch, select the entities you wish to copy into a new sketch.

In Tools -> Sketch Tools select Create Sketch from Selections.

Instantly, a new sketch will be created with copies of the selected entities. Upon opening the new sketch, you will notice that it does not have any references to the original sketch. The two sketches are independent of each other, in fact, the original sketch entities have not be deleted or replaced in any fashion.

Something to note when using the Create Sketch from Selections tool. You must select the sketch entities prior to selecting the tool, otherwise you will receive the following message:

There’s Plenty More To Come…

Make sure you come back next week for even more sketch tools. A word of advice: I understand that is difficult to get used to using new tools, especially if you have been doing things a certain way for a number of years. I highly recommend you try some of these sketch tools right away in your daily usage of SolidWorks. The more you use a tool the more you will find ways to use it. Some things you have been doing for a number of years can be streamlined by using tools you were unaware of before.

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