I am very new to SolidWorks (just went through tutorials), and I could really use some help modelling a crown-like jagged cone.
I want to make this in 3D:
I already figured out how to make a hollow cone, make a tangential plane and use the Wrap tool to make a sketch and use it to cut the cone. Here's what I have so far:
My problem with this is that I can't do the curved surface projection in my head accurately. I can draw my sketch on the tangential plane, but I have no idea how to dimension and distort it, so that when it gets wrapped around the cone, it will constitute exactly one half of that cone. With this method it seems that I'll either have to do A LOT of trial and error and then end up with an inaccurate model, or I need to do some 3D geometry transformations on paper so I can calculate the exact parameters for the sketch. Both seem like a lot of work - there's got to be a better way!
Any suggestions would be appreciated!
create a sheet metal cone model with
Answered with a tutorial: https://grabcad.com/tutorials/noob-question-how-to-model-a-jagged-cone
AttachmentsPart2.SLDPRT, 290 KB
Altug, thank you for your help! Unfortunately, I could not open your example file. I am using SW 2013, and it tells me that it cannot open a "Future Version" file. Could you please save it in another version, or maybe STEP format?
with ...step and iges format
I'm adding a new tutorial.
Answered with a tutorial: https://grabcad.com/tutorials/noob-question-how-to-model-a-jagged-cone--1
Altug, thank you for taking the time to make such a detailed tutorial! I learned a lot from it, although I did not end up doing my model using Sheet Metal.
I was able to use your tutorial to get something very close to what I wanted to do, but in the end I was not sure how to fold my part so that it is ready for 3D printing (I didn't actually want that gap that we used to convert to sheet metal).
Instead I ended up solving the problem by figuring out the angular pitch of the teeth, dividing the base of the cone into sectors for every tooth with construction lines, constructing tangential planes for the deep and shallow tooth, using a normal extrude cut, and then using Circular pattern and Mirror pattern to place the rest of the cut outs. This method also has the advantage of straight lines in the sketch resulting in straight lines of the cuts, whereas with the sheet metal approach I kept getting slightly rounded edges on the teeth.
I want to show you a technique I used recently in one of my models - Pi fruit bowl. It's quite simple.
First I extrude a cylinder, then wrap text or line and finally cut-revolve it in the desired shape - e.g. bowl, glass, cone.
Here is a step by step guide and the SW 2014 file.
I hope it's helpful.
Answered with a tutorial: https://grabcad.com/tutorials/noob-question-how-to-model-a-jagged-cone--3
Attachmentscrown.SLDPRT, 457 KB
Interesting approach, Plamen. Can you think of a way to do exactly the same on a cone rather than a cylinder, while still keeping the teeth straight? i.e. How would you correct for the conical distortion of the lines in your sketch?
The first thing that comes to my mind is to use the Flex command and straighten the teeth of the shown model.
I'll give it a try and let you know of the result.
Hi , try to explore the wrap function , you should find solution with it.
This function is able to project a curve aroud a cylinder or cone, and remove material. If you draw a baseline with lenght equal to circumference of the intersected cone, you have to draw your geometry on this line and remove material with wrap function .. Read SW help and "courage"
wrapping is done with the process.
This method is suitable for the production of the piece......
"This function is able to project a curve aroud a cylinder or cone, and remove material.".???
*You can do all kinds of drawing cutting process
*You can experiment by changing the sketch of the cut-and-extrüzyon2.
Thanks, Patrick. I spent a lot of time playing with the Wrap function, but I could not get it to work for me. The problem is the conical distortion that happens to all the lines of the sketch, so straight lines are no longer straight once they get wrapped onto the cone. I think it would be easier with a cylinder, but with the cone it was just too hard to figure out how to draw the sketch lines, so that the teeth would end up with straight edges.
Do you have any ideas on how I could have solved this problem?
I was able to achieve what I wanted with a different method though. I made individual Extrude Cuts for the deep and shallow tooth, and then used Circular Pattern and Mirror Pattern to make the rest of the teeth.