Cannot Select Center Point for Coil

[neljoshua]

I am trying to create a spiral feature.  I have seen some helpful tips here.  The issue I am having right now is that I cannot seem to select the center of a feature to locate the coil.

If I create the component/body on the origin, I can select the origin as the center of the coil.  If the component is located elsewhere, I cannot get it to snap to the center of a circle.  I have tried creating a construction point and also making a sketch with a projection of the circle.  Either way the coil center does not snap to the point I created.

Am I doing something wrong or is this just that hard?

[neljoshua]

Here is a quick Screencast.

[SaeedHamza]

Hi,

The center snap should work fine

Check this screencast

Regards

[neljoshua]

@SaeedHamza,

Thanks for the reply.  I see that it works for you.

Is there a snap or something that I missed?

[laughingcreek · Accepted solution]

it's an "infered" snap.  You have to hover over the edge of the cylinder first to tell fusion you want to use it for placing your point.  then as you move out to the center you'll see a dashed line following the pointer, and finaly a square when your at the center.

edit.  nevermind. it doesent work on my machine the way your screen cast is showing.  do you have "auto project geometry on active sketch" turned of in your preferances, that would change this behaviour. 

[TrippyLighting]

Yep, that would be the problem! Yet another one with the coil tool! And I've come across this before.

The coil tool is implemented as a semi parametric tool as it shares some of the same problems as the other primitives.

For a parametric CAD software the coil tool is simply not acceptable!

[neljoshua]

@laughingcreek & @TrippyLighting,

I do indeed have "auto project geometry on active sketch plane" turned off.  I do not like the way that Fusion projects things like this; there have been situations where Fusion has projected a complex surface with many more sketch entities than I wanted in the first place.  Fusion also does not leave a good record of what is projected.

Turning this feature on does indeed allow me to snap the coil to the center point.  This also explains why I can never get a hole to snap to the center of a feature (hence why I have always relied on sketch geometry).  Thanks for the tip!

Now, maybe someone at Autodesk can answer the following questions:

1) Why does"auto project geometry on active sketch plane" work, but actually creating a sketch does not?

2) Why does creating a construction point not work?

3) Totally separate question: where does this auto-projected sketch geometry go?  It always seems to disappear, and I do not like the idea that it is floating around out there somewhere.

[SaeedHamza]

Regarding your second question, it's not just about the point, in fact if you want to create anything using a sketch to snap to, it won't snap to that sketch unless the sketch is turned on, I mean if you finish the sketch and then try to create the coil by snapping to it, it won't work, but try creating the coil by snapping to that point before you stop sketch and it will work

Regards

[SaeedHamza]

About your 3rd question, the auto projected geometry is at the same place as the place it came from

For example, if you create a line by snapping it to an edge, a line will be created overlapping ( at the same place ) over the edge you snapped to. You can hide the body of the edge you snapped to in order to see it

Regards

[TrippyLighting]

When you start creating a primitive, such as a coil, cylinder, sphere etc. you will basically create a sketch. When creating a sketch in Fusion 360 - the primitives are no exception here - In order to be able to snap to geometry it has to be first projected into that sketch. However, when creating a primitive you cannot manually project anything into the sketch when creating primitive as the primitives skip a step and require you select a stat point.

Say for example you want to create a regular cylinder in that same spot you want to us e a primitive. If you have that preference turned off, you can click on Sketch and pick the plane. Then you can still use Sketch->Project to project something to snap to into your new, still empty sketch.then you can pick your circle tool and will be asked to pick the center point of that circle and can snap to that projected geometry and create the circle and extrude it.

When creating the cylinder as a primitive, the tool skips through a couple steps and you're immediately put in the state that requires you to pick the center point. You don't have a chance to project anything unless that preference is turned on, which auto projects "stuff" into the new sketch when you pick the face to place the primitive on.

Once you've created that primitive and at the latest when you click OK, the sketch is discarded/deleted/eased with anything in it!!!

So while the size of the primitive is parametric and can be driven with a user parameter, the location of the primitive is not parametric. That's why I called the primitives semi parametric.

Even as a Expert Elite I find this confusing. Something is either parametric, or it is not.

However, @jeff_strater would it not be possible to override the said preference setting for the creation of primitives ?

[neljoshua]

@TrippyLighting,

Thanks for the clarification.

[Reivaxy]

Hello

This was never fixed, right? 

I keep trying to create a coil centered on a point on my schema, but if a dimension update moves the point the coil stays where it was which of course breaks everything.

And editing or moving the coil does not even allow to move its center back to the new point position...

[laughingcreek]

if you need to parametrically place a coil, easiest thing is to create it in it's own (sub)component, and then joint the component into place.

if on the other hand you need to extract the helical path from a coil, there are other ways of creating a helix these days.

[Reivaxy]

Thanks for suggesting the sub component workaround. I'm using coil to create a custom thread.

[vincent8]

Hi,

I had thew same thing.  My Snap to Grid was off.

[fundamental4]

I solved in the same way! My "Snap to Grid" was disable.

[TheCADWhisperer]

@fundamental4 

I most definitely would not use snap to grid.

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

[fundamental4]

Hi @TheCADWhisperer 

please see attached file.

[laughingcreek]

would be simpler and achieve better surface quality to use a simple sweep without the coil. see attached.

[fundamental4]

Definetely @laughingcreek , much much simpler. 

thank you.