extrude profile missing

[Anonymous]

I went back in my timeline to edit an extrude by selecting 'edit profile sketch'. after I'm done, i got this extrude warning that profile reference is lost:

Warning: Extrude3
<b>1 Reference Failures</b><br/>The profile reference is lost, try editing this the feature to reselect the lost profile.

I then tried to edit the feature but I cannot select the sketch profile anymore. The picture shows what it looks like when I tried to reselect the new profile (still the same sketch)

strangely, when I went into the sketch i found that I could no longer highlight the profile by moving my cursor inside the perimeter. I checked the connection points to make sure there's no leaks or intersection anywhere, but it still doesn't work. To clarify, what I did earlier in this sketch is to scale the original profile, superimpose a spline, and delete the original profile. The new profile has much fewer control points.

I don't want to share the whole design file. If this description is not enough, can someone at least tell me what are the possible reasons why this warning occurs? Frankly last night i nearly lost it out of rage and frustration because I could not even edit a simple extrude. I think we can really use a database to explain the common causes for those warnings. If there's indeed one, I didn't find it.

Thank you.

[chrisplyler]

First, while you are editing the sketch, make sure that the Show Profiles setting is checked in the sketch palette.

Second, try bisecting your desired profile with a few lines, dividing it into a few smaller areas. Do some of those smaller areas shade in and others don't?

Use the above method to narrow down the problem location. Then try using the Coincident restraint on pairs of endpoints that you think are coincident but may not actually be.

xtn

[davebYYPCU · Accepted solution]

Edit sketch, select all articles then Right Click, if there is a menu item for

Move to Sketch Plane 

then your sketch has become a 3d sketch.  Move them by selecting your original plane for that sketch, and untick 3d sketch in the sketch pallet.

if not the case, divide and conquer should show you where there is a problem.

Might help...

[mavigogun]

Great advice given here already.   Add to that, Fusion may not recognize points as co-located that seem such; White Points usually indicate this condition, Black (or no points) connected.   The add-in Connect-the-Dots is an invaluable tool for connecting co-located points- I highly recommend it.