2D Sketching defining issue

I've followed the instructions precisely twice now incase the program was glitching and confirmed Fusion 360 is up to date. However my sketch is not fully defined. I'll attach screenshots below.

Any thoughts on this?

Referencing a similar post in this forum by Robert Deerson and answered by Connor, a solution to this problem was to "Fix" 2 of the Blue 45R lines, will attach a screenshot.

Any feedback is appreciated

Hi Edwin,

Its hard to say with these kinds of issues without seeing your process every step of the way.

If you export the file as a .f3d and attach it here, I'd be happy to have a look and see where the issue may be occurring.

I "Unfixed" the 2 lines as mentioned above so it is now back to its undefined version and exported for you.

Cheers

Okay, so in your particular instance, I found the outer arcs had lost their center point constraint. The equals constraints were doing their job and keeping each arc the same radius, but the actual position of those arcs had no constraint.

For me personally, I find the easiest way to find unknown unconstrained points in a sketch, is to simply click and grab a point or line that is unconstrained and drag it in any direction. You'll quickly see how things move to get an idea what isn't constrained. You can try adding certain constraints like a dimension similar to how I did in the video attached. If the over constrained sketch dialog appears, that particular constraint isn't the issue and you can narrow it down to what area is unconstrained.

Constraints can get particularly messy after using the trim and fillet tools because it isn't always clear what constraints have been lost. I have had experiences where very similar tasks have lost constraints in different ways which may be why you've experienced this even when following the lessons step by step.

To solve your example, all that was needed as shown in my video, was to constrain the center point of each ark to the center of the sketch. You can do this with the coincidental constraint on the arcs center point, to the center of the sketch or center point of the inside circle. You can also use the concentric constraint on the edge of the arc, to the diameter of the center circle.

Hope this helps, I've had some unusual missing constraint issues in the past and I understand how frustrating they can be.

That worked! Thank you

Out of curiosity though

Utilizing the "Fix" constraint and having it fully define the sketch, is that an issue?

Glad to hear it worked for you.

Not at all. The fix constraint definitely has its place and is very useful. You do need to be mindful when using it, because the sketch wasn't constrained by a more definitive way, there is the potential to accidentally move a sketch line or point by an amount that may not be noticeable. Then when using the fix constraint, you're constraining that part in the wrong spot and may not be aware of it. At the end of the day this still may not cause any real issues for the particular project you might be working on but when designing parts where tolerances are crucial, those tiny errors can cause bigger problems down the line.

I would say it's more about building habits that avoid the possibility of more errors. By constraining to key points or dimensions, you can be more confident that the final results will be what you were expecting.

Thanks legend