Impossible to create sphere in position

[Anonymous]

When I create a sphere it forces me to place the sphere in a new, blank sketch, which is useless because there is no way to reference the things I've already laid out in my sketches.  It only snaps to the blank sketch grid.

I already made a sketch and placed a point where I want the sphere, but it won't let me create a sphere on that point.  I don't understand how this is supposed to work.

Also if I click edit feature, there is no way to select a different initial point for the sphere.

Also I know I can move a sphere after creation using Point to point, but then this doesn't get updated if i alter any sketches parametrically.  Moves are not recorded parametrically.

[PhilProcarioJr]

One way you can do it is to right click on the sphere and make it a component, then make sure your sketch with the point you want to locate the sphere parametrically with is visable. Create a joint and select the center of the sphere then select the point in the sketch and the sphere will snap to the point. Now if you move the point in the sketch the sphere will move with it. I hope this helps.

[nabarun.paul]

Thanks @Anonymous for reporting the issue.

I see you are facing couple of different issues.

1) Not able to place the Sphere in some particular sketch plane.
- You should be able to place a Sphere in any plane
   a) either by directly seleting a plane
   b) or by selecting the sketch plane by selecting the sketch itself.
If you are not able to place Sphere in some particular sketch it could be either because of a particular workflow or could be because of issues with the model/sketch itself.
Would it be possible to share your model?

2) Not able to place the Sphere at some particular location.
- Looks like a bug with some special model. Ideally, one should be able to place at a point wherever he/she selects.
Would it be possible for you to share the model you are facing issue with?

3) Not able to change center of sphere while editing through timeline
- Will take up this issue with the team.

4) Sphere is not moved parametrically when the center is moved by editing the sketch.
- Will take up this issue with the team.

Please correct me if I misunderstood something.

As mentioned, if possible, please share the model (with little explanation of your workflow, would be helpful) with us for further analysis.

My Email Id is : nabarun <dot> paul <at> autodesk <dot> com

Thanks,
Nabarun (Fusion Development).

[Anonymous]

Thanks for your reply Nabarun.

Regarding your issue 1), selecting any given plane is not an issue, I can choose any plane I want.  The issue is that the placement of the sphere cannot be linked to any existing point in the model or sketches.

Your summaries of issues 3) and 4) are correct.

I have attached a simplified use-case for what I'm trying to do.  All dimensions are referenced with named User Parameters.

In the project I created a simple face in Sketch1, then extruded it to create a solid body.

Then I created an offset workplane from Sketch1, and started Sketch2 on this new plane.  I projected the centered point from Sketch1 into Sketch2, and draw a sketch point there.

Now, I want to create a Sphere at this point in Sketch2 and Join it with the existing body.   If I try to create a Sphere, I can select Sketch2 as the plane, but as soon as I do that, I look at the Browser and see that I am not really working in Sketch2, but that it has created a temporary Sketch3(it is temporary because once the sphere is created, Sketch3 vanishes).  Since this sketch is completely blank during sphere placement, there are no points to select.  I can place the sphere anywhere on this grid, but it will not snap to the point in Sketch2.  It may appear to be in the same location as the point in Sketch2, but if Sketch2 is altered parametrically(for example click Modify -> Change Parameters and edit the value of "Height" user parameter), the sketch point is moved but the sphere does not follow.

What I would expect to happen for sphere creation is:

1) If a point is visible then I can simply select that point as the sphere center without going into sketch mode at all.  

2) Also without creating an extraneous temporary blank sketch.

3) Any parametric changes that would move that point's placement would also affect the sphere's location.

I hope this is more clear.

[nabarun.paul]

Thanks @Anonymous for the explanations and raising the concerns. 

Thanks @PhilProcarioJr for the suggestion.

And also sorry @Anonymous for the troubles that you are facing. 

We are in discussion on this matter. 

For time being, as a work-around, I can suggest you following things. 

1) To create a sketch at some particular point, here are the steps: 

- select a Sketch where the point lies in. 

- go into edit mode by editing it

- invoke sphere command

- now you should be able to select the point to draw the sphere

(Please watch the screen cast for more details.)

2) for making it parametric, one way could be to do what @PhilProcarioJr suggested. 

Thanks, 

Nabarun

[nabarun.paul]

Hi @Anonymous, many of the issues (related to your workflow) are already on the list (but, for time being, I cant give any timeline when that will happen)

Thanks, Nabarun. 

[Anonymous]

It's apparent that Fusion 360 doesn't let you parametrically locate a sphere and I have a similar problem. I tried something like this starting with a cylinder but it has the same issue as the sphere, so I'm guessing that this gap is deep in Fusion 360's logic..

Here's a workaround you might find usable.  It involves:

Create a sketch where you can parametrically locate the sphere. 

At the target sphere center point; create a circle with the sphere diameter.

Extrude symmetrically the circle half the sphere diameter.

Fillet each end-edge of the cylinder by half the sphere diameter.

Voila!

I've attached a demo file.

Thanks and hope this helps.

[saccade]

Four years later, and this is still broken...just replying in the hopes it remains on the active bug list.

[etfrench]

Probably because it's ridiculously easy to create a sphere in any location desired using the Rotate tool and a joint.

[HughesTooling]

The primitives in Fusion are pretty useless and only useful for quick experimentation. For any accuracy build them from sketches, example for Sphere below. The primitives should work like the hole tool where you can pick references but there are lots of other more important improvements and bug fixes that should be worked on first!

Mark

[J.C.jones]

6 years and it still isn't possible to snap the centre of a sphere to existing geometry other than a plane. Sad.

[TheCADWhisperer]

---

@J.C.jones wrote:

6 years and it still isn't possible to snap the centre of a sphere to existing geometry other than a plane. Sad.

---

I can place a sphere at virtually any location that I desire.

True statement for me 6 years ago, and true statement for me today.

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

[etfrench]

Doesn't seem too difficult to joint a sphere to any location desired:

[J.C.jones]

I included a f3d in the attachment demonstrating the problem, screenshot here below. The goal is create a sphere at the highlighted point in the sketch using Create > Sphere.

Expectation: tool snaps center point to existing points like geometry, sketches or construction geometry.

What actually happens: tool asks first for a plane - I select the sketch - and once the plane is selected I cannot snap to elements in the sketch. I also cannot snap to construction geometry intersecting the sketch. I also can't help but notice that the tool temporarily creates a new sketch (that I can't edit) which is deleted once placing the sphere. I also do not seem to be able to edit the center point of the sphere once it is placed.

I too can think of all sorts of other ways to create or position spheres, but that kind of defeats the purpose of the desired simplicity of the Create > Sphere tool.

Note that this also appears to apply to Create > Box, Cylinder, Torus and Coil (haven't really tested Pipe).

[g-andresen]

Hi,

It's a bit tricky but it works.
1. click in the sketch > cursor appears
2. cursor over the point > click

günther

[laughingcreek]

@g-andresen -it's not snapping to the point in your vid.  it just looks like that b/c you have grid snapping turned on (you can tell from the blue box around your cursor).

if you select a planer face of a body (instead of a sketch) and if you have the evil "auto project geometry on active sketch plane" selected in your preferences, then the sphere will snap to edges and vertices of the geometry.  It snaps but won't be constrained.  so it's position won't update with changes.  ie, it's not parametric.  

you can get it to behave in a parametric way using a method already mentioned above, putting it in a component and using a joint to position.  But honestly, the primitives (as currently implemented) are mostly useless for parametric design.

[g-andresen]

Hi,

Thank you very much for the tip.

I saw the tip to do it via the component, but it was currently under the ice again for me.

günther

[etfrench]

Create the primitive sphere anywhere in space, then use the Align or Joint command to position it. The Joint command will allow it to be parametric.  I can't imagine the 4 mouse clicks needed will seriously affect your workflow.

[etfrench]

Just for grins, here's a primitive sphere aligned to a 3D spline at an arbitrary point on the spline.

[J.C.jones]

I caught on to this method in the meantime too and I suppose I will make do with it.

However, the issue as originally reported six years ago still exists exactly as the OP described it, which is a bit disappointing, especially considering how simple it should be to fix and affects an arguably very elementary tool.

@nabarun.paulif you have any updates about this, then I am all ears😉