Is there an easy way to find the centre/centroid of a face?

[Anonymous]

Hi all, 

I find myself wanting to find the centre of faces that are irregular polygons or have a mixture of curved and straight sides, and I am wondering if there is a better/easier way to find the centre of these faces rather than drawing a bunch of lines and doing lots of maths. It has been suggested to me to use the align tool to find the centre of these faces however I am wanting to use the faces as references in a sketch rather than wanting to align components together.

I came across this tutorial on how to easily find the centre/centroid of any face in Inventor. Is there an equivalent method of doing this in Fusion 360 that is this quick and easy? I would love a method that I could use on virtually any shape.

[TheCADWhisperer]

Place a work point?

[Anonymous]

Could you please give me a bit more information? I can create a point from the sketch menu but that doesn't snap to the centre. I'm not sure what you mean. 

Edit: Please let me know if what you meant is what I have marked as a solution or if there is a better method.

[wmhazzard · Accepted solution]

I don't think you snap a point to the center of an irregular face but you can use the measure tool and select show snap points, that will give you the center of the face and you can get the coordinates from the measure tool. Then place a point using those measurements. 

[Anonymous]

Thank you, I think that is going to be the best solution.

[daniels220]

There actually is a way to do it parametrically, though I have yet to test how robust this is to changes in the timeline. Make an offset plane from the face and choose 0 as the offset. The origin of any sketch created on that plane will be the centroid of the face. You can drop a sketch point there, and if necessary exit sketch and project that point back into another sketch with a more convenient coordinate system.

[laughingcreek]

@daniels220 - the underlying algorithm for locating the origin of a sketch placed on a face is unfortunately not as straightforward as that.  That it"works" in some simple examples is purely coincide.  once things start getting skewed around you'll find the origin is not longer placed  at the centroid. 

[daniels220]

Oh, that's too bad. Seems like it's still a worthwhile trick to remember in the cases where it does work, but good to know it's not reliable.

Is the actual algorithm for determining the origin, and axis directions, of (sketches on) faces and construction planes documented anywhere?

[HughesTooling]

You can snap a joint origin to the centroid of a face. So a workaround would be create a component, turn it's origin on and add a joint between the component origin and the point on the face.

Now you can project the origin into a sketch. Or use the XY plane from the component for your sketch.

[HughesTooling]

It does seem to be parametric and move when the face is edited as long as the point that shows for a face with the measure tool is the centroid?

Edit. So with a bit of testing it's not the centroid but the centre of a bounding rectangle.

[pcunneen874]

Reserving an old thread… I wrote a script for this. It allows you to select one or multiple faces, choose whether you want fusion to create one sketch for each or all of them in one go, and how it’s calculated.

[pcunneen874]

Oh and here is the script: https://github.com/BuildByAnyMeans/FusionScripts/tree/main/CenterPointOnFace