Confusion about chamfers: what distance am I actually specifying?

[JetForMe]

I wanted to chamfer a slot to allow a flat-head screw to sit nicely in it. I have a little guide that tells me how deep it needs to be (an M5 screw is 3.1 mm from the top of the screw head to the start of the shaft).

The Fusion chamfer amount is shown in two different ways, both appear to be wrong (there’s a third indicator that's correct).

First, it shows an arrow pointing into the chamfer, perpendicular to the chamfer face. This implies that the distance specified in the box is the distance from that face to the original edge, along the normal to it. This is not correct.

Next, in the chamfer properties, it shows a small icon with a blue highlight, which implies that the length of the face from top to bottom is the specified size. This is also incorrect. Another possible interpretation of this icon, consistent with the sketch colors for constrained and unconstrained geometry, is that the distance is the horizontal and vertical edges. This is close, although really it's the distance from the original edge.

Having written this post, I'm more comfortable that this is what is intended, but I think the UI could be refined to show it more intuitively. I know it's hard to cram the detail into such a small view, but it might be worth making the rows taller for this.

 

[Drewpan]

Hi,

The chamfer command is fairly straight forward once you understand what it tells you.

The arrow points to the face you are applying the chamfer to and can be moved in and out.

In this example the chamfer is set to equal distance and so I have moved the arrow perpendicular to the edge I

selected and the chamfer is 15mm from the edge on both faces.

If I set the type to two faces then I get a second arrow and they point to the direction I am moving the edge to

create the chamfer. In this case I am moving one edge down 25mm and the other edge in 15mm.

When I change to distance and angle, the arrow points to the distance from the original edge and I have set the

angle of the face to a constant 30 degrees. The icon near the arrow changes the angle manually.

I can always select one or more edges to apply this to and automatic select tangent geometry means fusion will try

to apply what you tell it automagically to all edges. If any one edge fails then it all fails. Not selecting this means it

will only apply to the edge you select. (Not 100% sure about this last point).

Flip is only useful for different distances and simply changes the face it applies to.

Corner type is just telling fusion what to do with corners.

So. In a nutshell what the arrows do change depending on what you are telling fusion, and measurements come

from the distance from the edge you started with.

Cheers

Andrew

[johnsonshiue]

Hi! The blue arrow is the manipulator allowing to adjust the chamfer width. The actual distance value you are specifying is the offset distance the participating faces will move.

For example, in your case, the vertical slot faces offset (enlarge) 3.2 mm. The Chamfer top edges are the intersection of the top planar face and the offset slot faces. Likewise, the top planar face offsets (lower) 3.2 mm. The Chamfer bottom edges are the intersection of the offset top planar face and the original slot faces.

Many thanks!