topic unable to select a profile to sweep in Fusion Design, Validate & Document Forum

unable to select a profile to sweep

Jaeger1787 — Wed, 13 Apr 2022 18:18:21 GMT

After a hiatus I am returning to something that is bugging me. I need to create a sweep along the lower edge of the cab shown here. I have drawn two profiles to be swept. One works excellently. The nearer profile can not be selected at all. I have checked the coincidents, dims and angles and planes. As far as I can tell the sketch is fully defined.

Where is the source of the problem?

Secondly why is the first valance profile showing yellow?

Re: unable to select a profile to sweep

jhackney1972 — Wed, 13 Apr 2022 18:35:57 GMT

When you created your sketch, you snapped to a point on the frame that threw you sketch off of the sketch plane. It is basically a 3D sketch so you cannot use it for the sweep. Take a look at the Screencast.

Re: unable to select a profile to sweep

HughesTooling — Wed, 13 Apr 2022 18:36:39 GMT

I don't think the profile is flat. If you Zoom in on this view you see the profile is twisted. You'd be better off creating an offset plane then sketch on the plane rather than end up with a 3d sketch.

You get an angle between these lines.

Re: unable to select a profile to sweep

HughesTooling — Wed, 13 Apr 2022 18:42:49 GMT

If you right click the yellow warning sketch and select review warning it will tell you what's wrong. You might have deleted something or an edit might have consumed the face you sketched on. You should fix these sort of errors straight away so you know what you did. Trying to fix it later or fix someone else's error can be difficult if you don't know\remember what broke it.

Re: unable to select a profile to sweep

Jaeger1787 — Fri, 15 Apr 2022 15:28:05 GMT

Thank you Gentlemen. Both methods gave very acceptable results. Following Mr Hackney's video I corrrected the leaning sketch, re-assigned it and swept as required.

With regard to the second part of my query concerning an error message in sketch 'Valance profile', I am not managing to correct the error, although the sketch performs as required in producing the wanted sweep. HughesTooling stresses the importance of correcting errors as soon as flagged up. However, although I understand the error message, I do not seem to be able to redefine the sketch to another plane. Nothing pops up in the context submenu:

Ah! got there. My mistake was thinking that the sketch had to be open, when in fact it had to be 'finished'.

Many thanks guys. Now to post solution accepted without appearing to mark my own work......