Different configurations may create different features ID (in your case wall). Mate refers to feature ID and this is the reason for error message.
Just create a new mate for a new configuration and configure it: keep an old mate for a new configuration suppressed and suppress a new mate for old configuration.
A few guidelines when doing multiple configurations:
1. This should be considered MANDATORY: Fully define all sketches. That way, when a dimension changes you control what happens to the sketch shape! For the rectangular shapes, just drag a corner to be coincident with the Origin. For the Hook, you need more dimensions/relations. Make sure all sketch entities are black (instead of blue).
2. Do your mates in a logical order and use the absolute minimum number needed to fully define the part (no "-" in the feature tree). I think you have extra mates that cause conflicts. This will generate mate errors. 3 coincident mates is all you need for a single part.
3. Add the parts in a logical order of assembly.
4. If possible, mate a new part to only one existing part. Bottom is your fixed part and so should be your first choice for ALL other mates.. Make Side<1> the second part. It can be fully defined with 3 mates to the Bottom. Then add Front<1>. 2 mates to the Bottom and 1 mate to Side<1>. Same for Front<2>. Then add Side<2>. Make all 3 mates with Bottom. Make all 3 mates of Hook<1> and Hook<2> ONLY to Front<1>.
5. Hook is the part giving you mate issues. As Vladimir said, when you have a part with 2 configurations that are created by 2 different features, you have 2 unique parts (from an assembly mating perspective), so need 3 unique mates for each configuration. My suggestion is to use ONE base flange feature and just change the dimensions in each configuration. As per #1, the Hook sketch is not fully defined, so add relations & dimensions to fully define it for the first configuration. Then change the dimensions to get the other configuration.Now you only need 3 mates to handle both configurations.
Getting off-topic, I see 2 parts (Bottom & Side) were done in student edition, so your assembly is now flagged as educational. To fix that, create brand new Bottom & Side parts then create (from scratch) a brand new assembly (using the above guidelines).
Thanks guys. I tried all the suggestions but ended up having to re-do it all from scratch. We have over 50 different configurations so to re-do every mate would have taken a long time, not to mention re-doing all the dimensions in the drawings. Making new walls off the one common feature is what we did in the end, like you pointed out Bill. We had no mating problems, but are now dealing with Solidworks errors in the drawings for some reason. I have posted another topic on that point.
Ah that's excellent, thank you so much for that! I have redone all of the parts already, but I know to keep that in mind in the future.