Am I doing something wrong - or does fusion360 have a problem sketching

[Anonymous]

When I am doing sketches to base my models off things start to grind to a halt after I start putting in a few constraints.

I've created a model as a test

http://a360.co/2egjPkM

If I add a fillet to the one corner on that cross that does not have fillet - my computer takes 10 seconds to complete the action.  That is on a quad core i7 with 16 gig of RAM.

Am I doing something wrong with the way I am sketching or is that just what I have to expect when drawing?

(Note: that is a contrived model to show the issue - I don't really need 4 concentric crosses)

[jeff_strater]

Well, that is a fairly complex sketch.  You will have a better experience if you stick to simpler sketches.  We will investigate this model to see where the bottlenecks are.  My suspicion is all the equal constraints, but we will investigate.

Jeff

[Anonymous]

Jeff, so just to confirm - it is slow for you also and not just my computer?

I'd understand the slow down if I was changing one of the inside crosses - and then all the outside ones that have dependencies would need re-calculation.

I didn't understand why adding the one fillet on the outside would cause a re-calc.

[TrippyLighting]

Inside of using mirroring ad patterning and other sketch constraints, you should create a simpler sketch. Only 1/8 of the current sketch is needed.

Then you should move to solid geometry as soon as possible and pattern that. Much better performance in Fusion 360.

Don't apply radii in a sketch if you don't have to either. Use the solid modeling radius feature.

[TMC.Engineering]

@Anonymous

Try something like this, on something so simple I draw the base cross add fillets the use offsets in new sketches.  as @TrippyLighting mentioned there are other ways like patterning.  point is keep sketch simple.

[Anonymous]

@TMC.Engineering Timm, 

Thanks.  I did start my sketch as two overlapping rectangles and apply the symetric and equal constraints as you did.  I however trimmed the inside lines away which added all the extra co-linear constraints.  I can see that leaving the inside lines and creating a selection set for later extrusions will make fewer constraints.

I just didn't realise what I was doing was considered hard or complex, so was drawing my sketch as I would have drafted it on paper 20 years ago.  This is a render of what I am doing http://a360.co/2eGXQWT .  It is the first complete CAD model I have ever done.  After trying OnShape and giving up I watched about 100 hours of Fusion360 tutorials.  I then just dived in and started drawing sketches as I would draw them on paper and extruding and lofting everything from features on one sketch.

With respect to the offsets.  I tried that, but I could not get the inside radii on the crosses to all be equal.  You'll notice on the contrived sketch I intentionally made the outside radii start at 3mm and grow to 6mm and 12mm.  But all the inside radii stayed at 3mm.  I guess if I leave the fillet till the 3D extrusion bit can solve that.  But some of the fillets need to be in the sketch to have 3 tangent constraints.

@TrippyLighting, thanks - I have been using circular patterning, rectangular patterning and offsets for other parts of the sketch, but some parts have slight variations per instance, so I can't.

[TMC.Engineering]

@Anonymous

couple thought on the inside corners.  you could add geometry to the offset for the 3mm radius, this could get ugly quick.  or as you mention leave it off and add 3d fillets

[TrippyLighting · Accepted solution]

My post was referring to your cross sketch.

Below is my sketch creating the same geometry with some mirroring of solid features and the small inside radii were added as solid features. Then more mirroring of solid features.

Fully parametric, much less work, very stable and very quick to edit. File is attached.