Noob question: how to create a fully constrained hexagon?

[Anonymous]

Hi,

Only started diving into Fusion 360 yesterday and also a newbie to 3D modelling, so bear with me here 

I select sketch, choose a plane, draw a hexagon with the polygon tool, but no matter what I try to add as constraints I don't seem to be able to get the hexagon fully constrained. I would think that if the center of the hexagon is constrained, the size and one of the vertexes constrained to be parallel to another edge, that should be enough, but it just stays blue.

Perhaps a more general question is: if an object is not constrained fully, what is the easiest way to figure out "what to add" to constrain it?

I can share my model in here tonight, that will probably help!

Bram

[patilsm]

Hi @Anonymous,

Thanks for your post and Welcome to Fusion community.

Please check the attached screen shot for fully contained Hexagon.

First need to Center point, Second need the dimension and orientation need to fix for details go though attached screen cast.

Thanks,

Sagar

[Anonymous]

Strange, that sounds like I got it theoretically right, but I might have another problem I'm not seeing. Perhaps my center point is somehow not fixed.

I'll share my project tonight.

Bram

[ToddHarris7556 · Accepted solution]

Bram - 

You're asking the right questions, and it sounds like your center point is indeed floating, so start with that. There are 2 potential easy fixes:

1) Start with a fixed origin. If it's your first sketch, then the model origin should project in as a fixed point. If you're sketching on an existing face or workplane, just doublecheck that you're using a point that's projected in from something else. Check Preferences> Design > Auto project geometry on active sketch plane. It's not mandatory that you use this option, but if you do, then you'll have something fixed to reference when you start sketching. 

2) Fix the polygon center. I wouldn't say it's a best practice, but you could simply click the center of your polygon and then use the Fix/UnFix constraint in the sketch palette (looks like a padlock) to pin it down exactly where it is. (Better practice would normally be to use reference geometry of some sort, so that if you update your model, the polygon would move appropriately. The 'design intent' I imagine would be to have the polygon located relative to something else) 

In either event.... you're quite right - what you really want is to have the geometry completely fixed. When it is, it'll turn black. In order to fix your polygon, you'll need to pin down three things: 

a) the center point

b) the orientation (usually the easiest is to pick a side and make it horizontal or vertical, but you could also dimension a specific angle relative to something else, or just pick a side and Fix it as described above)

c) the side length. There are several ways that you might do this (the simplest being just dimension a side) but one way or other, you need to tell Fusion how long the side is.

[Anonymous]

Hey @ToddHarris7556

I guess then this boils down to 2 even more "noobish" questions:

1. how do I see that the center point is actually grabbing on to a reference geometry point and not -for example- the grid? I think the center of my polygon happens to coincide with a grid point. Are different highlight colors used to highlight geometry points?
2. The plane I'm sketching on not yet having anything to anchor to (i.e. nothing drawn yet). The point I should to anchor to is on another sketch plane which is parallel to the plane I'm working on, but not coplanar. How do I solve that? Is this where the "construction" comes in?

Thanks a lot for taking the time to explain these concepts to me!!

Bram

[TrippyLighting]

If you start your geometry at the sketch origin it is automatically constrained to it with a coincident constraint.

Ultimately you want your sketch to reference the sketch origin somehow either by adding constraints, and / or dimensions.

When line end points are black, they are fully constrained.

You can project vertices, edges from geometry and sketch objects from other sketches into your current sketch with "Sketch->Project/include->Project".

In case you have not done so, please watch the tutorials in the learning section, as some of these and many more details might be covered there.

[TheCADWhisperer]

With a polygon by itself you need.

Fixed center point (generally the Origin Center Point).

Dimension (generally side to side, not corner to to corner for even number sides, inside or outside circle for odd number sides).

And this one that everyone misses - a horizontal or vertical constraint on one of the sides (or some other relevant dimension or constraint).

Attach your file here if you can't figure it out.

[Anonymous]

In the end it did look like I was forgetting the dimension!

When drawing circles (for example) the dimension is already there when drawing, so I didn't understand I had to add a dimension after drawing with a certain size...

Thanks for all the help!

Bram

[ToddHarris7556]

Glad you got it sorted out - 

I wouldn't necessarily call this one of the Ten Fusion Commandments, but you might find it a really useful habit to get into -

As you're sketching, doublecheck constraints as you go by grabbing various points/lines/entities and just drag them. See if they behave the way that you expect. You don't have to check everything, after every command, but probably just before you click 'Stop Sketch', take a quick scan and make sure everything's black. Or if blue, at least intentional. Try changing a few parameters and make sure the sketch behaves the way you expected. 

Like I said, it's not a 'make-or-break' practice.... but it can save some aggravation down the road. 

[Anonymous]

There should be a book with those...!

That said, it was only yesterday I figured out that I have to do ctrl-click-drag to move points in sketches. 😉

/noob out!