Bogging down during sketches

[Anonymous]

Fusion 360 is bogging down while sketching, here is the scenario:

I import a jpeg and start a sketch, i trace the jpeg. Initially everything is fine but as I add more trace points I have to wait 15 second for each point I add.

It's like click wait .... click wait.... 

Anyone else have this issue?

[TheCADWhisperer]

Can you File>Export your *.f3d file to your local drive and then Attach it here to a Reply?

How many entities in a sketch?

Can you use several simplified sketches in place of one complex sketch?

Are you (auto)applying only Coincident Constraints, or are you also adding Horizontal, Vertical, Tangent....

[Anonymous]

Thank You for the reply!

Attached is the f3d file I do have multiple sketches i'm not sure about how many points in one sketch instance?

"Are you (auto)applying only Coincident Constraints, or are you also adding Horizontal, Vertical, Tangent."

I'm not intentionally creating constrains, I'm just trying to trace the image and extrude it into a 3D design.

Thank You!

P.S.

I have experienced this in many other sketches.

[jeff_strater]

Thank you for sharing the design.  We will investigate the performance to see what is the problem.  In the meantime, I would suggest splitting your single sketch into multiple sketches, all on the same plane.  You could do one for the box + the letters, and one for the outline, and maybe another for the outline of the creature.

Jeff

[TheCADWhisperer]

---

svanwhy wrote: 

Attached is the f3d file I do have multiple sketches ...

I'm not intentionally creating constrains, ...

---

I see only one massive sketch for Sketch1 in the file that you attached.  (I did not check the rest of the geometry.)

I was going to suggest turning off all auto-constraints other than coincident, but just realized that I do not know how to do that in Fusion.

I would certainly do this as multiple sketches rather than one massively complex sketch.

If I turn on the Visibility of the Sketch Constraints, the sketch itself almost disappears behind the constraint glyphs.

[jeff_strater]

@TheCADWhisperer is correct here.  What is bogging down your sketch is the sheer number of constraints in this sketch.  There are a LOT of constraints.

So, one way to improve your experience is to get rid of those constraints.  My guess is that you did not intend all those constraints to be created.

Then, you can use the CTRL key (CMD on Mac) to suppress creating new constraints.

Here is a video showing how to do this:

Jeff

[Anonymous]

Thank you everyone for your awesome assistance!

I am just learning Fusion and I guess I do not understand constraints, I thought I was just tracing an outline. How do I just trace without making constraints?

Again thank you

[jeff_strater]

Hi @Anonymous,

The trick to trace without constraints is holding down the CTRL key while you are drawing.

Another suggestion that might help with this particular task is to use spline curves instead of just lines/arcs (unless you have a good reason for wanting to stick with just those curve types).  This will let you trace a bigger portion of your image with a single curve (and splines also don't infer constraints like parallel/perpendicular).  The only warning I would offer with splines is to not try to do extremely large splines:  Keep the number of fit points to maybe around 20, then end that spline and start a new one.  Also, use as few spline points as you can get away with - keep them spaced out pretty well.

Hope all of this gets you moving in the right direction.

Jeff