Polygoon with adjustable amount of sides using circular patern

[Anonymous]

So I want to make a polygoon and I want to change the amount of sides/points it has through parameters.

Now for my work I use Inventor and there I would make a Triangle with equal sides and the right angle. Then I would make a circular pattern of the extrude and keep it in the same body. If the sides of the triangles touched, they would seam together.

So now I wanted to try and do the same in Fusion 360. In the circular patern box I selected the extrude feature, but they didn't seam together. But instead a different body is added for each instance of the pattern and the top face is divided.

So this isn't what I wanted. So I scrolled back in the history and added a new feature joined to the triangle (a rectangle on top of it). If I then scroll forward again. BOOM the triangles are joined together into the same body.

This is what I want but without the rectangle, but suppressing or deleting the rectangle makes the polygoon split up in different triangles.

Now my question is. Is this a bug or is supposed to be so? And does anyone know another way of making an adjustable polygoon?

I tried the combine command but if I raise the amount of sides above the original count , some of them aren't joined together.

[HughesTooling]

The best I can come up with is to use a sketch. See attached f3d file. And yes pattern and mirror should have an option to join, I think there is a request on the ideastation.

Mark

Edit To open the file use New design from file on the file menu.

[Anonymous]

Thanks, I guess you used a circular pattern in the sketch? But how did you extrude it then?  I tried this aswell but couldn't extrude, I think the loop wasn't closed automaticly. How did you work around that?

[HughesTooling]

The design is attached to my first reply, just download and use New design from file to import.

Mark

[Anonymous]

Yeah I had used that one. Just didn't know how you got it to work. But tried it myself and this time it worked for me to. Probably did something wrong the last time.

Thank you very much!

[jeff_strater]

Hmmm...  I tried this as well, and saw the same results if I tried to model this using feature pattern.  This seems like a bug in pattern to me.  I think that pattern should join the "sections" together into one body.  Let me investigate.

Jeff

[HughesTooling]

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@jeff_strater wrote:

Hmmm...  I tried this as well, and saw the same results if I tried to model this using feature pattern.  This seems like a bug in pattern to me.  I think that pattern should join the "sections" together into one body.  Let me investigate.

Jeff

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The trouble is you can't set the extrusion to join if there's no other body, if you try it changes to New Body when you click OK. You can add a body that gets consumed by the extrusion and set it to join and it'll work.

See attached file with 2 components, one works using a cylinder that's consumed by the extrusion.

Mark

[jeff_strater]

Yeah, that is the underlying problem.  Inventor has what we internally call a "smart join".  If the feature is the first in the design, "join" is interpreted as "new body", but the UI still shows "join".  Fusion doesn't have this (and needs it).  You can see this in this scenario:

1. create a sketch with an overlapping rectangle and a circle
2. create an Extrude, picking the entire rectangle and the overlapping area of the circle.  Choose "Join" as the operator type (that doesn't matter, it gets converted to New Body anyway)
3. create another Extrude, picking the circle, and also choose "Join"

Now, you cannot reorder the second Extrude in front of the first (because that first one creates the body, and the second one joins to it).  In Inventor, you can do that.  Now, that scenario is not all that useful, IMO, while the pattern issue described here is a useful thing to want to do...

Jeff