Selection Methods in SolidWorks

There are a lot of different selection methods available in SolidWorks for use in different situations. I’m sure I won’t hit them all here, so feel free to chime in and add to the list.

Select All. This just showed up in SW 2012, and only about 15 years late. Still, it’s welcome, and much needed. Access it by Ctrl-A, through the menus at Edit>Select All, or there is an icon for it (3 select arrows). By default in a part it selects all edges, but this will change depending on if you have any selection filters turned on. If you are in a sketch, it defaults to all sketch entities. In an assembly it defaults to selecting all parts.

Window Select. Window select typically follows the defaults of Select All. Or maybe that’s vice versa. If you window select in a part, it by default will just select all the edges. To get other items, use the Selection Filter (F5). Window Select does have another function, if you make a box from left to right, it selects anything that is completely contained within the box, and if you box from right to left, it selects anything that is within or crossing the box boundary. Works for parts, assemblies, sketches, and drawings, and in conjunction with the Selection Filter. You can also use this in the FeatureManager, not just in the graphics window.

Select Other. The first thing to know about this is that it sometimes show up on the context bar on top of the RMB menu, if you haven’t elected to disable those. So you may see the symbol without the words, and wonder what it is. When you have a bunch of things on top of one another, and you can’t access the one you need directly, the Select Other tool may be the best option. This one can be tough to get the hang of. Just right click at the point where you know what you are looking for should be, and SolidWorks will pop up a list, shown to the right. It might have several different types of entities on it. In the image to the right, it is showing faces and parts. You could also find curves, edges, sketch entities, bodies, surfaces, midpoints, and other stuff.

Invert Selection. You know, I have never used this option, although I think it’s brilliant. You start by selecting something, and then you can access Invert Selection through the RMB menu. Again, you can use it in many different situations. If you select a face of a part and use it, it will select all the other faces. If you select a face of a part in an assembly, invert selection will select all the other parts in the assembly. You can kind of see how it works. Very cool tool.

Select Tangency. Select Tangency is a RMB option, and is available for faces or edges. You can also use it in sketches. Sometimes it will show up in a different place within the RMB menu, and it is included with some features (fillet, chamfer, draft) under the Propagate To Tangent name.

Select Chain Select chain is used again from the RMB in the sketches to select continuous loops of sketch entities. You can’t use it to select construction geometry.

Select Loop. Each edge (on a solid body) is a member of two loops. One loop for each face that it is adjacent to. Notice the orange and yellow arrows in the following screen shots.

There is also a method for selecting an interior loop. For example, if you wanted to select all the edges around the irregular hole in the middle of the part show to the right, you could click the face, and then control click one of the interior edges. When you use this in conjunction with a feature like the Fillet, it makes some edge selection much simpler, but I think some people may be scared off because of a bug in this feature. Notice below that the selection box shows Face and Edge. I clearly selected a face and Ctrl selected an edge. Notice also that it previews the fillet as if it means this selection literally – a face and an edge.

The problem here is that the preview is wrong. When you accept the feature, it will only fillet the selection of the interior loop. And for a further bug, if you accept the above feature and then later edit it, the selection will only list a Loop.

The second image is just the edit of the feature created in the first image. This bug has been in the software longer than I can remember. Just remember that interior loops don’t have to be difficult. You could also make this selection using the other loop selection method, with the RMB, so it isn’t really critical, and the malfunctioning function could just be removed from the software without losing anything. So this bug is unnecessary in several different ways.

Select Partial Loop. This is one of my favorites. In part I like it because it’s obscure, and in part because when it works, there is nothing else quite like it. Let’s say you wanted to select a chain of edges around a face, but you don’t need the whole closed loop. So what you do is pick on the first edge, then right click on the last edge that you want, and select Select Partial Loop. Your right click has to be to one side of the midpoint of the last edge, so that it will select the edges between the first and last edges on the side that you right clicked nearest to. That’s worth a little video, I guess.

There are also a bunch of RMB edge selection options that are specific to open edges on surface bodies, such as Select Open Loop and Select Open Tangency. Select Open Loop is different from the other loops, because all other loops are around the edges of a single face. Open loop can include edges from multiple faces. Open Loop in this case means edges that are only part of one face. So, the inside edge of the opening around the face shield are edges that only belong to a single face. SolidWorks can also show open edges in a different color (Tools > Options > Display/Selection > Show Open Edges Of Surfaces In Different Color – the default color is a medium blue).

Select Open Tangency just selects a chain of tangent edges that only belong to one face.

Selection Manager. The Selection Manager is only used in certain types of features, such as boundary surface, loft, sweep, and it is used to allow you to select a group of edges and/or sketches/curves to use as a single profile for the feature. So you could select 4 edges that touch end-to-end as a profile for a loft instead of trying to make a sketch with those entities in it. This is only used in specific situations, but if you’re in those situations, you use it quite frequently.

There are more specialized selection methods such as available with the Defeature, where you can select items based on size. There is the Component Selection tool in assemblies (found at Tools > Component Selection), which includes Advanced Select, which allows criteria for selection.

What other selection methods do you use or do you wish existed?