Can't create a constraint between two sketches

[hahn.bak]

I'm new to Fusion 360 and have been using it heavily for the past few weeks.   One issue I've run into and just can't understand is why sometimes I can't constrain to features in other sketches.  

In this file I've done 3 things:

1.   sketched a large circle on the XY plane

2.  created a reference plane along the path of that circle

3.  created a sketch on that reference plane with only a single point.   

I'm only trying to make that point coincident with the large circle on the XY plane.   Fusion 360 won't let me.  Can anyone please tell me why I'm wrong to believe it should allow me to create this constraint?  

sorry and thanks a million for your consideration

[jeff_strater · Accepted solution]

you are correct - you cannot create sketch constraints between different sketches directly.  You can use the sketch Project command to project geometry from an earlier sketch into a later sketch, and create constraints between the projected geometry and geometry in the second sketch.

[etfrench · Accepted solution]

Project the circle to the point sketch.  Make the point coincident with the projected circle.

[hahn.bak]

thanks much guys.   

I feel as though I've created constraints between sketches numerous times thus far.   Are there certain situations where Fusion 360 will automatically project geometry for you?

[jeff_strater]

I took a look at your design.  I made a guess about what you are trying to do - you want to dimension between the intersection of the ellipse in "Circle on XY plane" and geometry in "point on the "Plane along the circle".   For that workflow, you would use the Project -> Intersect command to create the intersection point, then you can dimension between that and new geometry:

[Anonymous]

Thank you, Jeff!

I've spent hours over the last few days trying to resolve this dilemma in a loft application for a filament extruder cooler duct. 

Just what the Dr. ordered.

[therealsamchaney]

Just to be clear, it's impossible in Fusion 360 to create Sketch 1, then create a new Sketch 2, and within Sketch 2 create constraints that fully constrain Sketch 1?

This would be incredibly useful for 3D sketching. For instance, what if I want to create a dodecahedron but want to be able to define it's dimensions by the overall height (one pentagonal face to the opposing face)? If we could constrain one sketch from another later sketch, I could achieve this by first sketching a pentagon (without defining the dimensions yet), patching it into a surface, patterning those surfaces to create the rest of the dodecahedron, then finally creating a 3D sketch with a construction line connecting the bottom pentagonal surface to the top one and giving that line a dimension. Then I could drive the entire dodecahedron with that one overall height dimension. Otherwise, achieving this functionality would involve some very complicated geometric math.

[ritste20]

I can't say I've looked at a dodecahedron in some time but with all sides being equal you set the length of the pentagonal edge as a parameter and give it an arbitrary distance like 1", build the full surface body with each side as a component and find the relationship (percent of the height of the dodecahedron) to the edge length.

That should at least get you close, then update the length of the pentagonal side in the parameters and let the model rebuild. If you wanted to then, once you know the relationship, you could make the pentagonal edge length a mathematical function of a desired finished height and let fusion solve the calculated value.

Regards,

[ritste20]

See below. Build your model with revolute joints on the edges to allow the shape to close itself. The scale factor from edge length to desired height = 2.227.

This way you can just edit the height parameter and automagically get the desired result.

[therealsamchaney]

Yeah, I considered that but I like my designs to be exact as much as possible.

If Fusion had a way to create a parameter from resulting geometry, I could also achieve what I need, but that's not possible. The measure feature exposes dimensions from generated geometry but you can't interact with those data in any way. If you could save the length of an edge or the resulting angle between two faces or something like that as a dynamic parameter, it would open up huge possibilities. As it is though you can only drive geometry with parameters and not the other way around.