# More Top SOLIDWORKS Sketching Tips

Part 2 of how little shortcuts can mean tiny savings each time these tips are used but, over time, will add up.

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Part modeling in SOLIDWORKS is fundamental to using SOLIDWORKS. Every model begins with sketching. Here are more tips on sketching that may be of help, in addition to those provided in my first article.

### Shaded Contours (Introduced in 2017)

Save time and headaches. You can see when you have a closed contour by turning this feature on. Bonus—it’s easy to move these closed shapes.

This is a useful visual indicator that the shape you are sketching is a closed contour that’s ready for extruding. But this is also useful because you can click on the shaded area of the shape and freely move these contours around. This was a welcome addition to the toolset in 2017.

### Reload—Control Z but Turned to 11

Save time and headaches. When you make a mistake that even Control + Z (undo) can’t fix, you can use Reload to automate the process of closing and reopening the file.

Pro tip: Want to get out of a tough spot? From the File menu, you can use Reload. This automates the process of closing your file, pressing “don’t save” to the changes and opening it again. Use this as a last resort or a mega super ultra Undo.

### Pierce vs Coincident—Know the Difference

Improve your SOLIDWORKS IQ. Knowing the difference between the coincident and pierce relationships is important if you want to be a true SOLIDWORKS Expert.

All pierces are coincident but not all coincidents are pierces. Does that make sense? Basically, the coincident relation puts a point on the projection of a line. But that line geometrically goes on for infinity. You can see this in the example video above. The pierce point is the one point where the projection intersects the plane. So, it’s the coincident point but it’s the only place the line and the plane intersect. You can see in the video that the pierce point is fully defined and located at the intersection of the line and the plane. A practical difference is that if coincident positions your sketch geometry where you want it, then great. But make sure to use pierce when using sweeps.

### FeatureWorks on Demand

Save time and clicks. You can add editable features to dumb solids one at a time with this trick.

You have a Parasolid or step file, but you want to make a few edits. For this, I like to load FeatureWorks on demand. Here’s the trick. Just click on the geometry you want to edit and select “Edit Feature.” Doing this loads FeatureWorks, which automatically recognizes the geometry and creates sketches and features you can edit.

### Arc Dimensions—Going Off on a Tangent

Save time and headaches. With this trick, you can go beyond the default behavior and dimension your way relating to curves and arcs.

Get control over your sketching by going beyond the default behavior. The trick here is to know that pressing the shift key while dimensioning to arcs or curves will give you the ability to dimension not only to the center point but also to the tangencies of these curves.

### Constructing with Construction Geometry

Save time and headaches. All types of sketch geometry can be construction geometry or helper geometry that you can use to get the job done.

The only construction geometry that has its own command is a line. It’s called a centerline, but it doesn’t have to go in the middle or the center. It can be used anywhere as construction geometry. The same is true for all types of geometry, actually. Click on a sketch entity and use the button in the graphics area to convert it to construction geometry. There’s also a checkbox in the PropertyManger. It’s a toggle you can use for all types of sketch geometry that can change it from solid sketch entities recognized in features to construction geometry you leverage to help you complete a sketching job.

### Turn Snapping On and Off—You’re in Charge

Save time and headaches. Sometimes the default behavior can get in the way. Turn off auto snapping of sketch relations so that you can get the fidelity you need for sketching.

As you’re sketching, you’ll notice SOLIDWORKS provide references to help you construct your geometry. This can either be helpful or super annoying depending on what you’re trying to do. You can turn off this autosnapping by holding the control key. Letting go of the control key will go back to the autosnapping behavior.

Pro tip: A white reference is just a graphical indicator, whereas a yellow reference will be added to the geometry.

### Sketching—One Entity at a Time

Save time and clicks. Save a click or two when you want to sketch only one entity.

Out of the box, SOLIDWORKS creates lines like chains. You have to press the escape key to exit the command. But if you know this trick, you can create one line at a time. You click and hold to create a line. The first click places the first endpoint. Then drag your mouse to and release to add the second endpoint.

Pro tip: There’s a system option you can replace with “Single Command Per Pick.” This means the command will end after you’ve sketched your first line or first circle. No more hitting the escape key! But what if you want to draw multiple lines or circles? No problem. You can double-click a command and it will persist so that you can create multiple entities. Give it a try. You might like it. It’s not how I use SOLIDWORKS, but I knew plenty of great designers who love this option.

That’s it for sketching tips I wouldn’t want you to live without. One way or another, the common theme to all these is time-saving—either directly by saving clicks or indirectly by saving you from countless headaches and frustrations. The clicks saved will add up over a career of using SOLIDWORKS. It could be the difference between meeting a deadline or passing the CSWE exam.