sweep issue

[Anonymous]

Any way to work around if the 'sweep would create an illegal surface'? i guess the sweep self-intersects and fusion doesn't want to create the form. 

[davebYYPCU]

Do you have a profile to sweep, pics are showing me just path, until you show a profile.

Could be wrong.

[Anonymous]

Hi, thanks for the response. here is the profile... 

[Anonymous]

it doesn't sweep past a certain point

[laughingcreek]

sweep has a harder time the tighter the curvature is.  one thing to try is to put your path on the inside of the curvature instead of the outside.

It doesn't look like this is the problem here, but when ever you have a sweep problem you should check your path with the curvature comb.  splines sometimes have sharp curvature changes at the ends that aren't visible by eye, but are evident with the comb.

[davebYYPCU]

it doesn't sweep past a certain point, 

You have a change in geometry there, the short curve has to be (probably 3d) tangent.

Might help....

[Anonymous]

HI, the sketch is tangent to each other, how do i get to be 3d tangent? 

[Anonymous]

alright, thanks... I'll try putting the path inside of the curvature later tonight! 

[davebYYPCU]

Both curves in the same 3d sketch? 

Lines are blue, something not right there, would expect the coil to be purple.

Edit sketch, click one curve, then Tangent constraint, then second curve.

Might help...

[Anonymous]

Hi, yes they are both in the same 3d sketch. I broke the link with the
projected coil because I will trying out different things and wanted to
post a clean image.

[TheCADWhisperer]

Can you File>Export and then Attach your *.f3d file here?

[Anonymous]

sure, here's the file. apologises if it doesnt make sense, i was playing around././

[TheCADWhisperer]

First thing I notice is that your Profile and Path are in the same sketch - it would never have occurred to me to do this.  Can you Project the profile to a new sketch and convert the original to Construction?

Second thing I notice is that your Profile is not on a plane Perpendicular to the start of the helical path.  I often see this as a mistake resulting in long feature solve time and incorrect resulting cross-section.

[lichtzeichenanlage]

I had the same problem and I used a coil and a line at the end, too. I just did to sweeps and it was fine for me. The start of the 2nd sweep was the face of the first sweep.

[chrisplyler]

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@Anonymouswrote:

alright, thanks... I'll try putting the path inside of the curvature later tonight! 

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I think this might solve the problem.

If you have a profile of some width, and you try to turn a small radius, there is some limit beyond which the inside of the profile is actually moving BACKWARDS along the sweep, which of course is self-intersecting.

That's why correct tangency can sometimes solve this kind of problem too. Because if you DON'T have tangency, you've got two lines intersecting at an angle. And if you've got that condition, then the two inner edges of the sweep at that intersection will be self-intersecting.

Letting the path represent the INSIDE edge of curves/corners solves all of that.