fusion 360 terrible performance

[northforkind]

I have noticed this problem before but it never has got this bad.  fusion worked fine when I started the dwg but now it just freezes up every time I try to edit the sketch.  Trying to edit the first sketch.  seems like the more I add or edit the dwg the slower fusion would respond.  Is this my computer or fusion?  Don't have this issue with other cad programs.  Very Frustrating.  taking all day to do a simple job

[HughesTooling]

Fusion's sketch solver is not the most efficient and you're just trying to do too much in a sketch. Symmetry is the biggest performance problem, best practice is don't mirror sketches, mirror features\bodies. This is best practice in all solid modeling programs. The next big mistake is using fillets in the sketch, for each 4 sided feature in the sketch you go from 4 constraints to 6 constraints\dimension. Keep the sketch simple and add the fillets to the body. Last tip is you sketch is not constrained, not a single line or arc in your sketch is fully constrained, this add a lot of load to the sketch solver, a bit like building a house of cards, adding constraints is like gluing the cards.

Also are the 2 vertical lines supposed to be parallel?

Mark

[HughesTooling]

Here's a big problem with your sketch.

The what looks like vertical line you use for your mirror is not vertical so the sketch on the right is going to be at an angle! You can see the rectangle on the right is skewed.

Mark

[TrippyLighting · Accepted solution]

1. Don't mirror sketch elements. Delete one half and then mirror solid bodies.

2. Most of the small fillets are not needed in the sketch. Apply those as solid fillet features.

3. Fully constrain and dimension your sketches.