Hole alignment on different bodies

[Nurgak]

It seems the hole feature is currently very difficult/impossible to work with.

I wish to make two aligned holes in two separate bodies, with slightly different diameters. I cannot use one hole to reference the other one for some reason, the holes are on different bodies, but must be aligned.

Ideally I'd like to reference both holes to a sketch point, but that is impossible. However much I click on the "Select" button next to "References" it doesn't allow me to set anything, it simply deselects itself. The only way to actually set something is to move the blue dot in the center of the hole and only then I can reference to straight lines only. I can also "snap to a point", but that is not what I want, I need persistent references.

This means that on a parametric part when some major things change the holes won't be properly moved and the part will get messed up.

Is this normal? Why can't holes be referenced to another hole on a different body or a sketch?

SolidWorks has excellent hole aligning mechanism that is missing in Fusion 360, or I haven't understood how holes work in Fusion 360.

[jeff_strater]

There are a number of ways to do this.  You can center the second hole on the first hole center by dragging the hole center manipulator around:

Or, you can place both holes at a sketch point:

Hope this helps,

Jeff

[Nurgak]

Thanks for the response Jeff.

Unfortunately the first example doesn't work the way I would like: once you place the second hole and drag it to the center of the first hole the "references" field stays empty. My impression is that they are not properly linked. My part is pretty complex, hence the need to parametrise everything and properly reference one action to another.

In the second case you place both holes relative to a point that is on the same face/plane. I like to create "master sketches" to which I reference my "build sketches" afterwards. It makes it a bit more cumbersome at first, but it's easier to work with afterwards, especially in Fusion 360 as sketches are not necessarily linked to bodies/components. In the case of these holes it seems they do not attach to reference points that are not on the plane where they are created on, which is unfortunately the case in this particular project: I extrude parts symmetrically up and down, thus the plane remains in the middle of the part and the hole refuses to attach itself to the reference point. In SolidWorks it is possible to reference to elements that are out of the sketch plane for example.

My current solution is to cut holes using the reference sketches and then chamfer the holes to get the countersunk screw hole I need. I think the hole feature could use some polishing, it would be a really great asset if it was more flexible.

[davebYYPCU]

As I see it, If your Hole reference is in the Master Sketch,

it needs to be Project > Project to a sketch for the face of the hole, a small step to the required outcome.

Might help.....

[TrippyLighting]

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@Nurgak wrote:

..., especially in Fusion 360 as sketches are not necessarily linked to bodies/components...

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I have a feeling that you probably should review Fusion 360's R.U.L.E #1.

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@Nurgak wrote:

... I think the hole feature could use some polishing ...

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If you have a reference plane with a sketch on it with hole locations, but your 3D objects do not coincide with that plane, then you'll have to create a new sketch on the face that you want to locate your screw hole located on and simply project these points from the reference sketch into the new one. Then you can locate your holes there.

These projections will update when you update/change your  reference sketch.

Some things in Fusion 360 require a different workflow

[Nurgak]

Thanks TrippyLighting. Indeed I'm still getting used to Fusion 360, I tried to read up on best practices, but did not see the 2 rules.

I think I qualify for the exception, my "skeleton sketch" references all the "build sketches" that are later extruded into components. However, at some point the skeleton sketch starts to look like a rat's nest if the design is a bit complicated. Also I'm doing the work twice... I'll try to clean this up.

[Anonymous · Accepted solution]

@Nurgak

Interesting stuff! I try to learn from all these approaches.

Just to make sure that I got the right idea. I created a skeleton ("drive") sketch in the root component. Then I created the components and use "build" sketches (with projected geometry from the skeleton-sketch). To play around a bit, I created a "hole" as an extrusion of a circle and also a hole feature positioned at a point - just to try out several ways.

So now I can parametically change the position of all these "holes" (real ones and extrusions) just by changing the dimensions in the skeleton sketch.

Does this (roughly) illustrate your approach?

Manfred