Rosette 250818

[pittsallen]

Hello Fusion Forum,

A little hesitant to post this question because it exposes
how little is known about the software. But is written
'The beginning of knowledge is the recognition of ignorance.'

This is sort of a follow up to post marked 'Son of Panel Fit 250812'

Pondered how to create this object for some time before it was decided
to draft it the same way I would have made the form when carpentry work
was done by using a miter box to create six wedges.

So six lengths were made with the desired profile and then the
ends were mitered at thirty degrees to the length so the
wedges would come together at a sixty-degree miter.

Just now it was realized that perhaps a more efficient way,
instead creating six sketches for the lengths and the
sketches for the miter cuts, one wedge could have been
created and five copies made from the originals and
the Joint command used to finish the form.

A defect in the method used is that when an attempt was
made to Combine the six wedges into one form, Fusion
would combine five of the wedges but would not allow
the last body to combined with the five-sided body.

But perhaps there is an even better method for making
the model. Have seen similar things done with a Circle Pattern.
Could a Circle Pattern be used as a process?
Is there a better way?

Thanks.

Allen Pitts

[etfrench]

Sweep would be my first choice. One sketch with the profile and one with a hexagon.  Sweep path would be five sides of the hexagon.

Circular pattern will also work, but it would take a few more steps to complete.  Extrude the profile the length of one side (It can be the inside or outside length). Use the draft command to set the end angles. Circular pattern that through 300 degrees. Join the bodies. Combine/Cut the 90 degree section out.

[kacper.suchomski · Accepted solution]

Hi

Look at this (random dimensions)

[jhackney1972]

Attached you will find my attempt.  It is basically like what @etfrench suggested in the second part of his post.  I did not add any holes, I will leave that up to you. If you need help with how the model was created please ask.  I copied your profile from your first sketch in the supplied model.  

Edit: I added a second version which uses the first method @etfrench suggested.  Model attached.

[TheCADWhisperer]

@pittsallen 

Step 1. Always, always, always work with symmetry about the Origin.

Your first sketch should look like this....

Let's learn how to do this correctly.

Attach your new file with first sketch here - then we will go to next set of steps.

We will improve on the other techniques shown here and also examine a technique that reveals a bug in Fusion and how to recover from the bug.

[JamieGilchrist]

@pittsallen, it looks like you're well on your way with help here.  @kacper.suchomski showed you how to make some fillets on your model, which is a totally sound way to do it;  I'd like to offer up an alternative, however.
So here is my version of the model using the sweep method mentioned before. (I know some folks on this thread will chastise me for not fully constraining my sketches. Don't box me in, man! 😛)
So two sketches and one sweep, gets your base shape very quickly

For the Fillets I used faces instead of edges

the reason I like this method are 3 fold:
1. much less geometry to select than edges

2. faces in a CAD model tend to be more stable/permanent than edges (as a general rule)

3. because of this, your Fillet will (generally) be more stable and predictable, should an error/warning occur 3 faces is easier to trouble shoot than 30 edges.

The one caveat here is the top face-inside edges doesn't need the Round/Fillet, but you can't selectively omit edges from face fillets...

So I selected the fillet faces and deleted them

Voila, gone. And the edges "self healed"

My general rule is delete features or faces of feature (as in this case) "very sparingly" from your model.  There are situations (like this one) where it has little, but positive impact on your workflow. There are other situations where it can cause you all kinds of heartache with downstream modeling. Many of us know this from thousands of hours of CAD time, and the exact times to use or not use this method are very situational.

[TheCADWhisperer]

@pittsallen 

You should follow my step-by-step instructions.

[johnsonshiue]

Hi! There are several ways to create the model. Pick the technique you feel most comfortable with, which would be the best one.

Here is a solution leveraging parametric relationship. The programmable model is driven by "Sides" user parameter. Changing its value can lead to a different model. You may also turn it into a Configuration Design. The beauty of 3D feature-based parametric solid modeling is like an algorithm, replicable in any CAD tool.

Sides = 3

Sides = 6

Sides = 12

Many thanks!