I’m new to freecad, so far I made it this way :
Sketch a rectangle for the top surface, pad it, add filets for the corners. Then select to bottom face, make a new sketch, another rectangle, then a datum plane 40mm below, sketch another smaller rectangle, and make a loft between the two to create the bottom of the tray.
Now for the hole I made a rectangle on the top face and made a pocket with an angle.
Downside of this, the thickness of the walls is not equal. Ideally I’d like a 1.5mm thickness everywhere. And I’m not really sure how to proceed to make the separators inside the tray.
What is the most efficient way to do it? thanks
I would make the tapered main bucket out of a loft made of two sketches that describe the dimensions of the upper and lower extremities of the shape. This can be hollow; there is no need to put a hole through it with a pocket. The hole and outer walls can be part of your sketch.
Similarly do not fillet the corners with PartDesign fillets. I mean, you can if you really want to but you can just use Sketch fillets inside your sketches and then FreeCAD won’t incessantly break your fillets (and thus the model) any time you change anything…
Example:
If everything needs to be tapered, honestly I would use lofts for all of the vertical components. Make liberal use of the “carbon copy” sketcher feature to make construction lines out of your two master sketches, and then all the other sketches you make for the dividers, perimeter lip, etc. can automatically tie themselves to any dimension adjustments you make to the bin itself.
Example .FCStd file: here.
Edit: It occurs to me that you could also make the tapered tray body by making a solid loft with no hole in it and then using the Thickness tool on the resulting It solid. This would be mechanically simpler, but would result in not having sketch geometry of either the inner or outer wall (depending on which side you tell the thickness to be on) which might hamper future additions/modifications.