Hello Being a novice in parametric 3D, I am asking for your experience for a small cat kibble dispenser project. I would actually like to improve this template for my use both in terms of design and functionality : https://wikifab.org/wiki/Pet-feeder_:_distributeur_de_croquettes_Arduino_imprim%C3%A9_en_3D But for the moment I am stuck despite my research on the modeling of a shell around the distribution system. This shell, the sketch of which can be seen on the plan1, should in fact improve the stability of the dispenser and hide the electronics underneath. My question is how can I proceed to model my complex surface between the top of my tube parallel to plane1 and my spline of plane1 by covering the whole thing with a dome? Sincerely,
Also for the dome shape there is the insertion function > >dome function (or free form) after closing the sketch and a boss, after there is the "shell" function which will probably be useful to you,
Hello Concerning the revolution it is a solution that does not work after my tests: the top of the dome must follow the red line: For the dome and the shells, I'm trying to understand how these functions work. I'll try a few things with it. And the free form doesn't have the air available in my version of solidworks! Thank you for your answers in any case!
If I understand your message correctly, the objective is to dress the distributor's tee with a "body". For this kind of realization, I think that the surface of SolidWorks is more suitable for the definition of complex shapes than the volumetric. Then it means thickening the surfaces to access the volume.
I am not sure that the "pencil sharpener" shape that I have chosen finds favor in your eyes, especially since I have limited myself to defining an envelope, without providing access to the "box", nor its division into several parts, which will depend on the method of manufacture and assembly. But the geometric approach used can give you some clues, in particular the smoothing function that creates the general shape. Model defined with SolidWorks 2018.
Hello @m.blt I really like this solution indeed. I made a sketch pile for the smoothing shape but the last sketch 19 (plane 4) doesn't fit in the function, is it because of the lines in it?
No more pencil sharpeners, make way for the sketch of Darth Vader's helmet... ;o)
Some recommendations for treating your geometry... - It is the upper sketch (19), consisting of a circle and two segments, that causes the refusal to construct the smoothing surface. Generally speaking, this function expects several profiles, all closed or all open. Sketch19 is neither one nor the other, and a bit of both... - When looking at sketches 15, 17, 18 with a straight segment, it seems that you are looking for a flat front face, coinciding with the end of the tube. It is better to treat it separately, smoothing will not allow you to easily make the curved side shapes and the foreground in a single step. - In the same spirit, I propose to treat one half of the lateral surface, then to complete it with symmetry.
A tip for managing splines: if you haven't already done so, check the box "Enable tangency and spline curvature handles" in [Tools], [Options], [System Options] page, branch [Sketch]. It allows you to display these handles that help shape the splines, by playing with the orientation of the tangents and the curvature values at the waypoints. The same goes for the display of the control polygon, just below.
In addition to profiles consisting of sketches to define a smooth, you can create guide curves on a similar principle that constrain the shapes to be respected in the second dimension of the surface.
