How do I make this shape in SolidWorks?
I am trying to make the shape of the top cover of the grill, but I do not know how to start with it. How would you do this?
I am only interested in the top cover of the grill.
3 Answers
Something like this?
1. Right plane, draw a partial ellipse
2. Front plane, draw a horizontal line, and a 2 point spline. Adjust spline as needed
3. Top plane, draw a partial rectangle
4. Extrude ellipse sketch as a surface
5. Trim the surface with the Spline sketch
6. Reuse spline and rectangle sketches, or redraw them to form a "boundary"
7. Boundary surface to fill the gap. Be sure to set the contact with the Spline sketch as tangent to the front plane. Otherwise there will be ugliness when the surface is mirrored later.
8. Knit surfaces
9 Mirror twice about right and front planes
Continue as needed by adding more details, or converting back to a solid by closing off the "bottom" with a Planar Surface. Or by using the Thicken command.
There are likely more efficient ways to make the shape, but this is the first that came to mind.
Hey Uchenna,
FredSWUG's method is completely legitimate and works, but another way of doing this is to:
1.start a sketch with the ellipse tool and draw a line separating this into a half ellipse.
2.extrude this.
3.use reference geometry to ensure there is a plane either in the center or to the side of the shape perpendicular to the flat face of the shape.
4.sketch a corner cut out on each side on this plane
5.cut extrude.
If you want this to be hollow you can also use the shell tool.
What's the point of modeling this barbecue? It must be made in sheet metal. The procedure is quite simple, it is to have in mind that a sheet metal requires arcs of circles. If you want to know more, make sure you have to build it and not just model it in 3d. Interesting as a model it does not stop more than to see if it works well! :)
One of the unfolded faces in image 3.
