Simple Sketch that I Cant Fully Constrain
The Constraining of your Fusion model sketches fully is generally a very good practice. Trying to get the Browser Full Constrained Icon is not always something to worry about. In the attached Animated GIF I show the important geometry is fully constrained but the Icon is missing in the Browser. The reason is that I did not give either of the construction lines a length description. This makes little difference to the sketch but it prevents the icon from showing up in the Browser.
John Hackney, Retired
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When you have symmetry within the sketch, it is more efficient to draw a centre lIne, use diameters, where possible, fillet in the modelling window.
When revolving the chamfer could be omitted as well. Lazy efficient is a good thing.
When done right no black dots on boundaries, just arc / circle centers.
I suspect big black dots are where the problem lies, and be careful of overlapping duplicate lines, one will be fully constrained, but another would not be.
(Check the 3 - 19mm dimensions for the same lines)
For beginners, One sketch per feature is recommended, so they are much easier to constrain.
Might help...
I solved the problem by using construction geometries
If this is Sketching as a test example, then you can still clean it up a lot. (Advice not critical)
Highlighted in yellow,
You should not have black dots on any boundary that is not a centre point, Fusion hides all the points that are connected, (Coincident)
Use inclined dimensions as a last resort, (95 off the origin at an angle) The line coming down at 3 o'clock should be coincident on the circle, tangent and no dot.
The 14 and 26 dimensions on the left can be replaced with Equals Constraint, do one, make the others the same.
You have a 60 rad construction circle, and 120 diameter dimensions doing the same thing.
You also did the outside circle and then added over the top 4 arcs - between the bosses, (overlapping stuff is super hard to find when I didn't draw it)
You have a black point inside the right side hole - not on the original.
My oval highlight - 2 fillets where they are not needed, but if you are putting them in there should be 3. (Both ends of the 22 high line.)
and lots of angle dimensions that are duplicated.
You only had to copy the original. You have not been efficient, or lazy, yet. if making the part, it would be streamlined like this, because of the modelling tools.
Sketch origin should be where the dimensions come from, most come from the left side big circles.
The Hole Boss is the 2nd Extrude, the hole is on a centre point, Hole tool has lots of options to add countersink, counterbore and threads where needed on that same point.
Do one and let Fusion add the hard work with the pattern.
Might help...
