This is a little tip that those who are seasoned SolidWorks users probably already know, but that can be very useful for those who are not so experienced in “the art” of top-down assembly modeling (I’m not extremely experienced but I learned this one by hitting my head against a wall a few times). It’s also a very simple tip, because all you need to do is remember one thing:  the infamous in-place mate. 

Every time you create a new part in the context of an assembly, a special mate is added that will define the position of the new part in the assembly: an in-place mate.  This is true regardless of where you choose to place the new part’s base sketch: a plane in the assembly, or a plane or face of another component in the assembly. The following image shows the in-place mate between the part Rod Support and the part Rod, which was created in-context.

On one hand, this is a good thing because you don’t have to worry about mating the new component to keep it from floating around; it’s already been done for you. The tricky part, though, is that the in-place mate means the new component is fully defined, completely fixed, it can’t move or rotate at all.

This is important to keep in mind if you are adding other components to the assembly that would require this one component to move or rotate in order to mate correctly.  If this is the case, you are likely to see errors displayed here and there in the feature manager, you will get warnings about how adding this or that one mate will over define the assembly, and other mates will fail as well, but it’s not likely that you will see an error message or warning next to the in-place mate. Nevertheless, always keep in mind: in-place mate means fully defined, no movement whatsoever. So, if you really need that component to move, you are going to have to get rid of that in-place mate, otherwise it just won’t happen.

Once you decide to delete the in-place mate, you’ll get the following message.

What does this mean? Well, if you answer “yes”, not only the in-place mate will be removed, but also all the external references to geometry of other components in the assembly will be broken, as well.  In this case, you will have to proceed to dimension sketches in the component, then add mates in order to define its position relative to other components in the assembly.  Remember, once you break the external references, you can’t undo it and your component won’t automatically update when changes are made to the other components in the assembly that it used to reference to. Also, you can’t add an in-place mate yourself. This is a special kind of mate that is automatically applied to parts created in-context. On the other hand, if you answer “no”, then you get rid of the in-place mate, but you get to keep all the external references. You still have to add mates in order to place the component correctly in the assembly, but you can rest assured that your component will update when changes are made to the geometry of those other components it references to. Neat, huh? Now, keep it in mind. Not that your life depends on it, but it may come in handy one of these days.