Convert Entities tips (some of these tips can be used for much more …)

After you start the Convert Entity command and select the entity or entities that you want to convert, note that the cursor changes to a picture of a mouse with a green check mark on the RH mouse button in the pick. This is telling you that if you are finished making your selections, that you should simply right click and this will validate for you so that you don’t have to move your mouse all the way over to the property manager to do so.

Speaking of the property manager, when using Convert Entities, by default, the property manager dialog for it is pinned so that it stays open after you hit enter. When SolidWorks made this change many years ago (this command did not work anything like it does now back in the day), this fact that the dialog stayed pinned after we hit enter (or right mouse clicked) really annoyed us. So the key is to simply right click twice in quick succession. The first right click converts and the second one closes the command.

Note that in order for this right click business to work as far as issuing the enter command, you must do it before you move your mouse any distance. Once you move your mouse a quarter inch or whatever, this right click option goes away as you can tell by the fact that the icon changes from the mouse icon with the green check mark on the right mouse button to a regular arrow cursor.

When you know you are going to use the Convert Entities command, and you know that at least one of the things you want to convert is an opening with multiple edges that are tangent, the fastest way to get this done is to right click on one of the edges first and pick Select Tangency from the menu popup. Then when you issue the Convert Entities command your selection will be done for that opening.

If you don’t do it this way, or if the opening you want to pick does not consist of tangent edges, you will want to right click on an edge and choose Select Loop from the list. Unfortunately when you do the Select Loop the loop that it selects is always a face, which you never want, so at that point you simply click on the yellow arrow to tell it not to select a face but to select the loop of edges. Unless there are just three or four edges that you will be picking, it is probably quicker for you to right click one edge and Select Loop and then click the yellow arrow to change direction of the loop.

If you do want to pick the entities individually, or if you have round holes that you need to select in order to convert, I strongly suggest that you use your edge filter. If you don’t know what I mean by that, you are probably in the majority but you are missing out on one of the best and most wonderful things in SolidWorks. Press the F5 key on your keyboard to turn on the Selection Filter toolbar – or it might already be on and pressing F5 will turn it off. With it on, watch what is happening on that toolbar as you do the next step. Press the E key on your keyboard and you will note that the Edge Filter becomes pressed on the toolbar. You are now filtering only edges, which means you won’t/can’t accidentally pick a face when you were trying to pick that elusive edge. Press the E key again and it will no longer be pressed in. So the bottom line is when you use filters, you want to make sure to press the key that turns off this filter after you turned it on so that you don’t wonder 10 minutes from now why you are not able to select the face or vertex you are trying to select, or whatever. Also, while this wasn’t always the case, your cursor will have a funnel next to it to show that you have a Selection Filter turned on.

Trust me if you don’t use them, force yourself to start using Selection Filters.

(Note that you don’t ever have to press F5 to turn on this toolbar, you can simply press the key to activate or deactivate the filter, I only showed you this F5 so that you could see the filters and how they turn on or off with a keyboard press.)