Origin for 'Create' sphere does not snap sketch geometry.

[Swarfmaker]

A simple scenario. A single sketch plane with two intersecting lines. Exit sketch and 'Create' sphere. Select the plane of the sketch - OK; Then says 'Draw Point' - but that point will not snap to any place on the sketch other than the origin.

If during the creation of the sketch a point is placed, the sphere being created will not snap to that either.

If however 'Create Sphere' is selected while the sketch is still active, then it snaps to wherever I wish. Similarly if I go back and edit a sketch, then I can again place the sphere where needed.

The concept of only being able to create a 3D object and place it while in Sketch mode seems a little strange - although I realise that sketches are 3D also.

[Phil.E]

Hi,

Thanks for posting. This looks like it may be a new bug. (edit: it's not) I'm going to report it as such because a Primitive should be able to snap to things like sketches because they snap to points on bodies. I'll let you know what I find, whether it's as design or not.

And only to be clear, this is not the only way to make 3D shapes. Most shapes are made by sketching a closed profile and extruding, revolving, or lofting them. Primitives act a little differently, they draw the sketch and perform the 3D operation all in one command. 

Please let me know if this helps or if you have more questions. Thanks again!

[Swarfmaker]

Agreed that it is an un-anticipated behaviour, but the sphere is a useful primitive as it does not lend itself to generation from a sketch.

As it happens the toroid primitive behaves the in the same way as the sphere.

Thanks for your attention.

[TrippyLighting]

---

@Swarfmaker wrote:

Agreed that it is an un-anticipated behaviour, but the sphere is a useful primitive as it does not lend itself to generation from a sketch.

---

Sketch a half circle and revolve it. That'll get to a sphere.

If it comes to parametric behavior in terms of remaining snapped to a location the primitives in Fusion 360 are pretty dysfunctional.

[Phil.E]

To be clear: snapping is not associative. It never has been. This means snapping primitives, or snapping extrude distances. If you need associative geometry you must use sketch and constraints, or for extrude use "to object",  to make parametric relationships between sketches and model geometry.

My comment above was simply to state that I would expect a primitive to snap to a sketch like it snaps to a model body. Again, the snapping in this case is not associative and will not update if you go back in time to change the input for the primitive location. @TrippyLighting is correct to suggest using a sketch if parametric behavior is desired.

Please let me know if you have more questions.

[pdevDMGRW]

What's the point of using sphere then, if you can't snap it to a point?

In case anyone else has wasted an hour on this (like I have),  here's another golden rule:

DO NOT USE SPHERE TOOL.  IT IS USELESS.  DRAW A SKETCH CIRCLE AND ROTATE IT INSTEAD.

Bah humbug.

[turningGCH43]

Yeah, me too. Another huge waste of time trying to create a sphere at a sketch point.
Trying to place ball bearings percisely is a PIA

[jhackney1972]

I normally do not use the Sphere primitive but if you do, the Screencast shows how to position it both as a body and as a component.  By the way, you can use any vertex to replace the point is used for placement.

[zinefer]

This has also wasted a ton of my time. It's also made deriving a spring's location and size from a parameter far more work than it needs to be.

[sjnoble]

I just discovered this lack of snapping to a point drawn on a sketch.  Will only snap to origin.  I'm just going continue to sketch arc's and revolve.  Perhaps the Sphere tool hasn't needed to be expanded on with the programming dept. 

[vivian.morresey]

As a relatively new user who feels that they doing alright with F3D, gets stuck when changing parameters in the model, only to find that my process of using a sphere in a parametric process, still finds this short coming. The only positive is the answers above allows me to fix (arc with revolve) the issue so that I can move forward. I really thought my process on using the sphere, and trying to snap it to a projected sketch point isn't an unrealistic process... yet clearly not supported

[Phil.E]

Hi, thanks for responding. I'm curious what you are designing with spheres. Can you provide an image or screenshot, or just describe the design?

[jhackney1972]

Moved

[vivian.morresey]

Basically, making my own version of RAM mount inspired connecting arm. I used the sphere as the system is based on 1" balls, and was using that for both visuals (clearances etc) and then as a Cut tool into the bodys. I then wanted to make the arm length parametric to make different lengths as required, but the sphere wouldn't move with the sketch point.

I did use a arc/revolve and used a sketch point as the centre, which then moved everthing nicely when editing the sketch length (between two arc/revolve generated spheres).

 

[Phil.E]

Okay, makes sense.

The reason I ask is related to your design. I see that as 4 components. 2 bearings, and two halves holding them. If these are all components, the bearings would snap to joints that are parametrically driven. Your method is just as valid for something this simple. 

[TheCADWhisperer]

---

@vivian.morresey wrote:

 I then wanted to make the arm length parametric to make different lengths as required, but the sphere wouldn't move with the sketch point. 

---

@vivian.morresey 

Are you familiar with using Joints?

Can you File>Export your *.f3d file that didn't work as expected to your local drive and then Attach it here to a Reply and someone will demonstrate solution with Joints?

[vivian.morresey]

The level of work that I do is still relatively simple, and while I have had some experience using joints and multiple components, I don't use them much. In saying that, I am started to do more of multi-part designs, so will do some practise on your suggested approach. Thanks for the help.😀

[Phil.E]

I created a playlist with a couple tutorials for you on Autodesk.com/learn. They have short videos if you just want to watch, and data sets if you want to click along. Let me know if you would like more!

Assembly Basics