How to rotate a rectangle?

[Anonymous]

Surprisingly no previous answers or instructions on this simple situation. Maybe I'm running a deficient copy of Fusion 360. I just want to rotate a rectangle.

I've sketched it. Then in the same sketch want to rotate it. I call the Move command or keyboard shortcut M. I click on the rectangle, then click on the center as pivot point. But it does not rotate. In fact, it seems there are dozens of sub objects to click and I don't want any of them. I've tried marquee-selecting the entire area, and it shows "13 selected" but still won't rotate. See attached screenshot.

What am I missing?

[Inspections_JCH]

This is a hard thread to follow. As a new user, we are told by Autodesk in their tutorials on how to get started using Fusion 360 to place things at the origin. Now after struggling with this same issue of sketch rotation, we learn that we should never use the origin if we wish to do things that seem natural to us at any time in the future. What we need is a comprehensive tutorial from Autodesk on the "Good and Bad of the Origin." They surely thought the origin should have special attributes. Now is the time to give us a complete picture of how special it really is. It seems to me that we have been lead down the rabbit hole when we go anywhere near the origin.

I am creating a round object and after some work on the sketch I realize it will suit my needs to have the entire sketch rotated 30degrees around the origin. Even after reading this thread, I am more inclined to simply recreate the entire sketch than try to hunt down all the constraints that are not "intuitive to this user".

I am now in a situation where editing the sketch shows the sketch grid rotated. We need a comprehensive tutorial on the subject of rotating from sketch to model. And, before you ask, yes I have spent a few hours searching the help files for these answers. None of the material I have found yet is comprehensive on the subject of rotation.

Sketch grid rotated.

[etfrench]

The simplest way to rotate a sketch is to put it in a component, then rotate the component.

[Inspections_JCH]

@etfrenchHave you seen an instructive tutorial on this technique? And specific to my curious nature, as we begin a new project and then under that project, how is it we have sketches that are not in a component?

The answer to my rhetorical question is that it is specifically because Autodesk instructs us to sketch first. Now if they have a video that begins: "Create a component and then within that component create your sketch.... OK, we didn't follow the instructions. But at this point, I am still looking for the instructions for the most productive workflow that will facilitate and allow rotation of my sketch elements around the origin.

[etfrench]

See Rule #1.

You can move a sketch into a new component or subcomponent any time before a 3d model is created from the sketch. 

I haven't watched an instructional video of creating a sketch inside a component, so I made one for you.  This is the way I normally start a new file:

[TrippyLighting]

You should probably explain the need of having to rotate a sketch by sharing your model and maybe create a screencast.

[chrisplyler]

Ninety percent of the time, I only create a sketch inside of a component.

But occasionally, I want a sketch that is above any component in the browser hierarchy. This is when I want a single sketch that controls two or more components, AND those components don't need to be exported as stand-alone Fusion files for reuse.

The more you use Fusion for various projects, the more you will get a feel for the most suitable way to set up the hierarchy of a design to suit your needs.

[jefoid]

Why in the world is there no rotate command in a sketch?  By that I mean, select objects, pick a point, type in angle.  It's a 2D sketch.  How can this not be possible.  

Aside from that, how do I rotate a rectangle or better yet anything?  The internet is filled with tips and tricks regarding the creation of components.  Others say simple, do this... and of course it doesn't work.  How do I rotate a rectangle?  I can see the boxes where you can type in a rotation, but nothing ever rotates.  How can it be this hard??  

[davebYYPCU]

Generally we don’t rotate a sketch, it is put in the right orientation on creation. 

Use 3 point Rectangle, you get perpendicular and parallel constraining.

There are exceptions, but rotating a horizontal sketch to an angle, must have the horizontal and vertical constraints removed first.  (Obviously - but not intuitive)

That Done, Select the articles, and Move rotate will work.  

If one leg of the rectangle is not horizontal, you can dimension it to rotate to a new angle.

More complicated the sketch, the more constraints to remove.

More often after Redefining a sketch plane the sketch has most / all the constraints removed,

Rotated / mirrored by Fusion, then fixed, = green sketch articles, unlock them

and the sketch would have to be rotated, which does work.

Might help....

[etfrench]

Rotate is built in to the Move command.  Learn to use the software as designed, not how you think it should work😁

When a rectangle is created, Fusion 360 normally adds horizontal and vertical constraints instead of perpendicular constraints.  Simple change the horizontal and vertical constraints to perpendicular constraints and you can rotate the rectangle.

[HughesTooling]

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@jefoid wrote:

Why in the world is there no rotate command in a sketch?  By that I mean, select objects, pick a point, type in angle.  It's a 2D sketch.  How can this not be possible.  

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When you draw a profile in Fusion it tends to create one Horizontal\vertical constraint then it create parallel or perpendicular constraints. A sketch like this can then easily be rotated accurately if you just delete the vertical constraint and drag to rotate and add an angular dimension. This night not work too well if you make overly complicated sketches.

This profile was sketched in one go then dimensions added, as you can see a single constraint stops rotation.

Delete this and you can drag it around then add an angular dimension. Note I drew this away from the origin because snapping to the origin tends to catch out new users. If you fully dimension sketches you will never need the Move command!

[TheCADWhisperer]

@jefoid 

I think you should have started a new discussion thread.

The thinking is all wrong -think real world Component Degrees of Freedom (I stated Component - NOT Sketch).

What is your true Design Intent? Do you have a picture of something similar from the real world?

Can you File>Export your *.f3d file to your local drive and then Attach it here to a Reply?