I've tried searching similar questions on google but all the results I get either point to to making surfaces or lofts which I don't want. I've also seen people say you should use Boundary Boss/Base for it but all the tutorials I see use two different 2D sketches and form material between them where as I just have one 3D(doesn't really work when I tried it). I've attached some pictures of the part I am currently working on.
I've drawn out a rough 3D sketch of what I want the shape of that area of the model to look like. I've basically drawn out all the lines and vertices, and I just want the space enclosed by the 3D sketch to be a solid, as I intend to 3D print this later.
The already solid part of this model I basically sculpted made by sketching on a bunch of angled planes over rectangles and extrude cutting them to create the surfaces I have right now, but it's taking a lot more time than I can spend and is getting tedious and difficult to picture how to do.
Also, none of the faces in the 3d sketch are parallel.
I'm fairly new to Solidworks and CAD in general, so any help would be greatly appreciated, and thank you for your time.
What you can do is use your existing 3d sketch to drive a series of new 3d sketches, one for each planar facet. These new, planar 3d sketches will then be selectable for use with the 'filled surface' feature.
Once you have enclosed the volume with these 'filled surface' feature patches, you can generate the solid by selecting all of the surfaces and using the 'knit surface' feature.
It seems like a lot of individual features to get there, but because you can leverage the 3d sketch you've already created, it will go quickly.
You're on exactly the right track by creating a surface right on top of the extrude face. 'knit surface' is the easiest way to create the surface patch on the extrude face too, just select the extrude face and finish the command. But if you've already created a surface right on that face you don't need to create it again, and it probably didn't just disappear, it just isn't the default selection when you try to click it.
Near the top of the model tree is a 'surface bodies' folder where you can select all of the patch surfaces with ease. Alternatively, you can right click the solid and 'hide' it to make picking the surfaces easier.
You should be all set to generate the solid.
When you do you'll then notice a 'solid bodies' folder right above the 'surface bodies' folder and it should have 2 bodies in it.
You may want to 'combine' the original solid with the one you've just created to finish the model as a single solid body.
Thanks a lot!
I came upon another issue though. Working more on the part, I've made all the surfaces from my 3D sketch, but when I want to make them a solid, one of the faces for the solid isn't part of the 3D sketch; it's one of the faces from an extrude cut. So it looks like a 3D sketch that would form an enclosed volume except the 3D sketch is connected to a square face from an extrude as one of its faces. How then would I make a solid from that? I tried making a surface over the extrude surface but it just disappears and if I try to knit while selecting the extrude as one of the surfaces it doesn't allow the Create Solid checkbox.