How to select partial line/arc segment in sketch?

[esBB6UJ8]

In a sketch, I have created a complex line/curve defined by multiple tangent circles and lines.  I'd like to select specific intersecting segments that are part of the curve so that I can create a circular pattern from them.  I can do that by trimming all of the segments that aren't a part of the desired curve, but I'd like to keep all of the original primitives with their constraints so I can easily change them in the future as I tweak the design.  Basically I want the select tool to behave like the trim tool.  I've tried everything I can think of and searched using multiple combinations of terms without success.

[laughingcreek]

selection of sketch elements unfortunately doesn't work that way on fusion.  There are probably alternative workflows that will get you where you want to go, but with out a specific example any suggestions would just be shooting in the dark.

The words "complex line/curve" curve and "create a circular pattern from them" raises a red flag.  making patterns of simple sketch geometry is usually not suggested.  doing so with complex geometry is even dicier.   It's better to make patters using solid geometry features when ever possible.

[esBB6UJ8]

To add some detail, I’m creating what is effectively a pulley for a specific belt (GT2). The tooth shape and pattern is specified using multiple intersecting arcs with different radii. Given that the belt spec is for when it is straightened, I have some additional constraints in the design so that the pulley curvature matches the belt.  Fusion seems completely sketch driven for a design like that. I sketch a specific tooth based on the spec (along an arc around the pulley). Then I create a circular pattern from the segments associated with the tooth. I could replicate all of the segments / primitives, but that makes creating the selection for the extrude operation very tedious (there are 130 teeth along the pulley). 

[jeff_strater]

@laughingcreek is correct - selection does not work that way.  You can use Break to split a curve at a point, keeping both parts:

But that won't quite keep all the original geometry's constraints/dimensions.

Another possible approach is to use construction sketch geometry to draw the bigger curves, then trace over it with "normal" curves in the segments you need, using coincident and other constraints to lock the small curve segments to the construction curves.

[laughingcreek · Accepted solution]

for gear type objects it is really better to sketch 1 tooth, creating a solid from that , and then use  pattern in the solid modeling area instead of patterning the sketch.  Heavy sketches like that will bog down fusion and make things unmanageable.  plus it's easier.  

[esBB6UJ8]

Thanks for the advice.  That works *much* better than trying to create a large circular pattern in a sketch.  Which is more efficient: creating a new body from the 1 tooth, creating the circular pattern from it and then combining the bodies, or create a pattern from the face from the sketch and then extruding it with a join?

[laughingcreek]

I usually apply pattern in such a way that geometry is created already joined, rather than creating a bunch of bodies and combining after them after.  in the attached example I extruded a tooth with the type set to join.  then I patterned the feature so the result is also a joined single body.  this allows for the number teeth to be parametric.

[esBB6UJ8]

I've tried that and run into problems - apparently because of the number of teeth in the gear/pulley (130).  I'm able to extrude the tooth, and then select it as a "Feature".  But the "Adjust" option warns that there are "Too many pattern instances.  Consider using Optimized/Identical compute option".  When I try "Optimized", it tells me that the compute failed "Error: C-Pattern1 / Compute Failed / One or more pattern instances could not be intersected with the original body.  Try adjusting the pattern settings, or changing the selections."  It reports the same error even I decrease the number of copies.  When I try "Identical", it doesn't report an error, but it only adds two additional teeth (next to the original).

I did notice that when selecting the tooth as a feature, it does select the face of the hub of the gear/pulley as well.  If I select the wrong axis, I can see that its including that face in the circular pattern.  That's partly why I originally created it as a separate body, since I could select only the tooth for the pattern.

Even though I get an error for the "Adjust" option, it looks correct, so I'm going to try to go with that. 

[g-andresen]

Hi,

Please share the design for a better understand the real conditions.

günther

[esBB6UJ8]

Here it is.  

Thanks for the help.

[TheCADWhisperer]

Sketch1 should be fully defined before all else.

I also (almost) never repeat dimensions - I use equal (=) constraints.

Is there supposed to be any relationship between position of the inside teeth and the outside teeth?

[TheCADWhisperer]

I simplified your sketch just a bit, but otherwise - looks good.

[esBB6UJ8]

Thanks for the help everybody.  It is looking very good now.  I ended up parameterizing everything - including all of the specs from the GT2 belt itself and a formula to compute the number of teeth from the hub OD (which I had sized to contain an integral number of teeth and to be at least 2mm greater than the fixed hub ID).  I also removed all duplicate dimensions, so everything should be cleanly constrained / parameterized.  And ironically I'm probably at a point where its sized just right and I won't have to touch it.  But at least the design is clean and I learned more about Fusion and good design process.

For anybody that's interested in what I'm doing, I'm building an external / auto focuser for a small telescope (William Optics RedCat 51).  The focus ring effectively slides onto the rubber / knurled helical focuser on the RedCat 51 and a GT2 belt connects it to a stepper motor that is connected to a Raspberry Pi.  I have a separate (in progress) base to mount the stepper and rPi to the telescope.  Software runs on the rPi (Ekos / StellarMate) to drive the stepper to focus in concert with a camera.  Everything is printed on a Prusa i3 mk3, though I may have to get the mount machined if I can't get enough tension on the belt to drive the focus ring without significant / varying backlash.