This type of Sheet Metal can be created in two ways:
1.Adding Edge Flange to flat sheet metal or
2.Base Flang to a sketch.
Does it make any difference in next working?
Again it always depends on design intent and complexity of the model. For the simple U shape you show, creating the part using one sketch and one sheet metal feature would be the preferred method where I work. However if you find it less confusing to add edge flange to flat sheet metal then go for it.
Unless I'm making a large radiused piece that requires Insert Bends, I always start with a base flange and add each feature from there, even for "simple" sheet metal parts..
It allows for greater control over each feature, it doesn't bury features within other features and SW tends to behave better.
If you have mixed methods of sometimes incorporating bends into the base flange and sometimes not, model maintenance is greater, especially so when there's more than one person.
Not every part can be modeled with a multiple feature base flange, so I don't bother developing that design habit.
I would usually (but not always - depending on where the design is going from this stage) start with the U shaped sketch - much easier to edit dimensions.
Also - when I see users create Flange-by-Flange I more often see errors of keeping track of outside or inside dimensions (whichever are more critical to the design).
Well, the more I think about this the more I think about adding qualifiers.
Use the technique that makes logical sense for the design.
Only you know the finished Design Intent. (You haven't indicated the finished design.)
This video starts with flat sheet metal and adding edge flanges. Whereas I want to try it again with sketch and Base Flang. That is why I want to confirm it. First attempt failed, I want to try it again.
Solidworks in your Industry Pt7 - Sheet Metal - YouTube
I would go with Kevin's suggestion and that is how I usually do. As he has mentioned, it give more control over features down the tree and handle the design intent. For e.g. if you want to add flange on all four sides? Then you can simply edit the edge flange and add the two other sides
I always start with a base flange and add each edge flange one by one. As Kevin Chandler & Deepak Gupta explained it gives me more control over each edge.
We have our bend table for our sheet metal parts, but in some cases we need to go with K factor.
If I go with starting a base flange to a sketch (your method 2) I don't have control over each bend individually and in some cases I end up with not precise flat patterns.
Also if I add each flange one by one, I can control relief type & default radius of each bend.
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