Sketch geometry is over constrained issue

[kshea9RNL8]

Just when I make the mistake of thinking I may actually be starting to get a handle on Fusion 360 I draw myself into another corner and very quickly at that

Unable to get past even the most basic of drawings, every thing is another hurdle and so many things are tried one forgets how he even got to the present hurdle, just not clicking with me, that doesn't mean I'll be giving up though

When drawing a line from the inside top and bottom corners of the 1 1/2 SQ tangent to the large OD circle the lines are not equal length and they are snapped in place when I see the tangent icon.

When I check to be sure the circles are concentric (with the two tangent lines deleted)  I get an error that the "Sketch geometry is over constrained" which is confusing because I don't see any constraints and do not recall applying any.

Pic and file attached, unable to do a screen cast with out getting a "Windows Aero Theme disabled" with no success in finding a solution for that, at least none that worked.

[TheCADWhisperer]

I would always set to capture design history.

Your two circles appear to have a coincident constraint a the centerpoint which means that a concentric constraint is not needed - that would be redundant.

[HughesTooling]

What you've probably done is pick the origin when you drew the circles and that will automatically create a coincident constraint, some but not all automatically created constraints are hidden.

If you click and hold the mouse button down on the centre circle centre point you will get a selection menu like this.

When I select the point highlighted then right click the selected point I get this menu with an option to delete the coinsident constraint. If you delete it the circle will be free to move.

Mark

[kshea9RNL8]

Do not want to inject more confusion with capturing the parametric time line, don't need it right now.

Thanks for the reply

[kshea9RNL8]

I get the selection menu as shown in your first pic, how do you know which sketch point to select in the list, there are 5 and two profile.

Tried all the sketch points but do not get the option to "delete coincident constraint"

Wish the screen cast worked, could be selecting things in the wrong order.

[HughesTooling]

Hide the other sketches and you should end up with only 3. There's no way to know at the moment to tell them apart, I have this suggestion on the Ideastation at the moment, vote it up please as the more votes the quicker we'll get it.

I think the points are listed oldest to newest so the point at the bottom of the list is the origin the next the circle centre, not sure why the top point in the list is there, maybe you've draw something then deleted and the point was left behind.

Mark

[jeff_strater]

Thanks for the great response, @HughesTooling,

One point:  It should not matter which point you select to choose the "Delete Coincident Constraint" menu item.  It should be available for both points.

I took a look at the design, and I think the reason why there are three points at the origin is because there are multiple sketches in the design, and Select Other will show any visible points.  If you hide all but the sketch you are working on, you should only see two points there.  Leaving other sketches visible when you are editing a sketch can be confusing, especially if they are co-planar.  In general, I prefer to have just a single sketch on one plane, to avoid this confusion.

As to the fixed origin point...  I personally dislike that particular feature of Fusion, so I tend to avoid using that point in my sketches if I can avoid it.  I voted against that behavior, but apparently other popular CAD systems do that, so we were getting feedback that Fusion needed to do this as well...

I, personally, would like some additional sketch debugging tools to be made available.  I'm not sure exactly what those would be, but something to help untangle your sketch when you have lines on top of each other, and to find which center point goes with which circle, etc.  Hopefully someday...

Jeff

[kshea9RNL8]

Guess I tried all but the right one , think you are right on the sketch point order, selected the very last Sketch Point and that provided the "Delete Coincedent choice"

I see when constraints are applied it creates secondary construction lines, don't recall that, is that new?