Polygon Radius and Sides Defined by User Parameters?

[DESKTOPMAKES.COM]

Having trouble creating a polygon that is defined using parameters and can be updated simply by updating the defined parameters. Appreciate any insight into doing this.  See the attached screencast to see the problem I'm having.

Thanks,

Vladimir

[HughesTooling]

The number of sides created by the polygon tool is not parametric, you can control the radius by adding a dimension after the polygon's created. If you want a fully parametric polygon you'll have to construct one something like this, file's attached. It uses a circular pattern.

Mark

[TrippyLighting · Accepted solution]

The polygon tool in the sketch environment is not really parametric, however it is very easy to create your own.

[TheCADWhisperer]

It is (almost) always advisable to pattern features rather than sketch entities (a sketch polygon).

A parametric solid polygon (feature pattern) is trivially easy.

This question routinely comes up on all of the parametric MCAD forums.

[TrippyLighting]

Yes, but just almost. What Fusion 360 is missing in the solid patterning UI  is a join option, because patterning 6 solids will leave you with 6 single bodies and not just one.

You'll have to use the combine tool to combine all of them into a single solid.

If you then reduce the number of sides the Combine tool in the timeline will create an error and turn yellow, if you want one more side than you'll have to update the combine feature in the timeline manually.

[TheCADWhisperer]

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@TrippyLighting wrote:

...What Fusion 360 is missing in the solid patterning UI  is a join option, ...

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Ah yes, I keep forgetting this inexplicable omission. 

Maybe someday the Fusion developers will "walk across the hall" and talk to their Inventor colleagues at Autodesk.

Somebody should add this to the IdeaStation.

Hmmm, I think I will create a new kind of car, a crazy California idea, all electric. Maybe I'll call it an "Edison".

But no air conditioning, no heater,... ... 

[DESKTOPMAKES.COM]

Thanks Mark, really appreciate the file.  It really helped me out.

-Vladimir

[DESKTOPMAKES.COM]

Thanks Peter, exactly what I needed.

[Anonymous]

 @TrippyLighting

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@TrippyLighting wrote:

Yes, but just almost. What Fusion 360 is missing in the solid patterning UI  is a join option, because patterning 6 solids will leave you with 6 single bodies and not just one.

You'll have to use the combine tool to combine all of them into a single solid. 

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There is at least one exception. If you patterning a feature, which has join option in it (for example, Extrude with join to another solid), the pattern result will be also a single body.

[Anonymous]

Except when I'm trying to pattern an extrude that's joined to the "main" body it's also taking that "main" body along with the extrude itself, e.g., I'm trying to create a number of pegs on the top of a plate. I extrude a single peg and join it to the plate (I need to fillet it). If I attempt to pattern that extrude (with the number of pegs being parameterized) I get the pegs, but the plate is also patterned, which is definitely not what I want.

That is poorly-described; sorry. Think of it as a comb: each tine has a width, the space between the tines has a width. The tines need to be filleted against the handle.

[HughesTooling]

Can you select the faces rather than the extrude and pattern? A screen grab will show us exactly what you're working with or can you make an example you can share as an f3d file.

Mark

[Anonymous]

Because it's joined the top faces of the tines are joined to the handle.

I ended up working around it by extruding the handle separately, then
extruding the first two tines and filleting them to the handle, then
patterning the features [extrude, fillet].

Interestingly, while the body was shown being also-patterned out, it was
*not* present after the pattern was completed: it may have worked with what
I'd tried originally, but I abandoned it thinking I'd have a bunch of
"extra" handle w/o tines on one side of the comb. So immediate problem
solved, although it's a lot more work than it needs to be.

(I'm not making a comb 🙂 But for all intents and purposes, it's a comb.)

[TrippyLighting]

As someone who participated in this thread get notifications of new posts.

I would consider patterning tools one of the most essential core tools of any CAD and in general 3D. modeling tool.

It is interesting to me that this thread was started more that year and a half ago and nothing has happened to these tools and they are still so unfinished.

There are number of tools in Fusion 360 where is almost feels that the goal that was set for implementing the tool fell utterly short of anticipating the very next set a user would have to make to compete a task.

It is simply a fact that there are a number of circumstances where you end up with a body that needs to patterned and then joined to something. Any time after the join operation the quantity parameter is changed the combine command either does not combine all the patterned entities, or it breaks because a previously combined entry is missing.

That same applies when a component is patterned and joined. Patterning bolts isn't exactly an unusual task in mechanical engineering 😕

More complete pattern tools are in pole position on my 2018 Fusion 360 Christmas wish list. 

[Anonymous]

Completely agree: this is no-brainer functionality. It took me nearly an
hour to figure out how to make a parameterized comb FFS.

[emmagolson]

this creates and inscribed polygon. is there a similar way to create a circumscribed polygon?