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Help: design approach suggestions

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Hey all,


I'm new in this forum and quite fresh in Solidworks I have a part which I want to model (screenshot of drawing attached), and I feel that this should be done using the Sheet Metal features. However, I cannot figure out the correct approach for making this part. So far, I have made a simple bracket (top-down view) and don't know how to add the geometry of the front plane, as well as the angled part of the bracket.


Could someone with more experience help me get on the right track? I do not want the entire part done (that's what I'm trying to do ), but only guidelines for the correct approach.


Sorry for (probably) noobish questions, but any help will be appreciated!






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Hey Paul. there are several ways to make the angle geometry.

1. You can draw the part as a solid(not thin wall) and convert it to sheet metal. There is an interesting notch on the back of the angle part that would have to(most likely) be done as a cut after it is sheet metal.

2. You can draw the sides(draw one and mirror), then make a jog or flange between them.

3. Start with the angled face first and work your way out.


If you start with the angle face you can sketch just a line and use the Base Flange/Tab feature. give it a thickness value and then do Dir1 as a Mid Plane extrude out .555". After the feature is created if you select the feature in the tree, then select the blue dimension on the screen(.555) you can add the tolerance values in the model. or you can do that at the drawing level.When you create your first Edge Flange off of the angled piece you want to press "Edit Flange Profile". There is a minor problem here in the face that the coordinate system isnt the same as the model. it is based off of the edge of the body you started with. So you will have to add angles and delete constraints this way. As you can see this gets a bit complicated.


The way i would likely do this is to create an offset plane, draw the sketch profile of the side(before the radius) 1.379 long with the right end at the 74.5degree angle. Mirror this body and then create an Edge flange. When making the edge flange make the inside edge of your original part the first selection and then the inside edge of the mirror part the second selection. I would need to play around with this a bit because the way that back end bends is critical. The flange position will likely be "outside" or you will have to do some custom work to make sure there isn't a weird relief.


That is a pretty general overview of a few ways to do it. If you want more specifics i can give the part a try for real. Attached is a SW2015 file showing the two methods I elaborated on. Just note that there are many different ways.

Sheet Metal Help.SLDPRT

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