Sweeps on 3D sketches

[Legrand]

Before I put my fist through my monitor... I know this can be done, as I have done it in the past, but I'm apparently not remembering the special "trick" required.

I have created a 3D sketch, starting at the origin. I then create another sketch for my profile (a circle), again using a plane through the origin. I then hit the sweep function, pick the circle for the profile but every time I try to pick the 3D sketch as the path, nothing happens...

Any ideas?

Thanks...

 

[TheTick]

Measure the distance between your profile sketch plane and your path curve. There might be a minute gap which makes it not possible. This shouldn't preclude selecting the curve for a sweep path, though.

Check your filters to be sure. Perhaps try filtering for curves only. That, and try picking the 3D sketch from the feature tree.

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[Legrand]

The path curve is coincident with the origin and the profile sketch was done on the "Right" plane, which passes through the origin. There is no gap there.

I have also tried to pick the 3D sketch from the tree as well... several times...

No filters help...

Thanks for the suggestions though...

 

[CorBlimeyLimey]

Are you highlighting the "Path" selection box before selecting the 3D sketch path?

Try pre-selecting both the profile & the path before activating the Sweep feature.


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[ctopher]

Try creating the circle sketch first, then the 3DSketch.

Chris
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[SBaugh]

If the profile cuts into itself it will not follow the path and fail. try making the profile smaller to see if that the case.

Regards,

Scott Baugh, CSWP
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http://www.3dvisiontech.com

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[Legrand]

I had tried reordering the profile before the path, that didn't work, and neither did changing the size of the profile (circle). I went all the way down to .001" with no results.

 

[SBaugh]

IS the 3D sketch actually in 3D space? If it's not then it will not work.

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Scott Baugh, CSWP
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[ctopher]

Legrand, I have that size monitor and res, still is havoc on my screen. As Scott suggested, it may be sutting into itself. It may be to small to see or find. Or the radii are too small.

Chris
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[Legrand]

It is not cutting into itself, as I have tried several different profile diameters.

Not quite sure what this means though: "IS the 3D sketch actually in 3D space?"
How could it not be in 3D space?

 

[SBaugh]

Well how did you make the path? Did you use a line or a spline?

http://www.scottjbaugh.com/Images/Spline.wmv

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

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[dsgnr1]

remember to exit your sketch before using the sweep feature.
sounds simple, but went through it today with an associate.

¿)

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[Legrand]

Scott: I used a line, moving from one axial view to another (i.e. from X to Y to Z), so it should be in 3D space then... I think...

dsgnr1: I can't exit the sketch via a sweep, it will only allow me to exit via an extrusion... what does that say about my "3D sketch"?

 

[CorBlimeyLimey]

I can't exit the sketch via a sweep, it will only allow me to exit via an extrusion

Huh!

remember to exit your sketch before using the sweep feature.

The Profile & Path must be seperate sketches.

Both sketches must be exited from (using the sketch icon) before activating the Sweep.

The Path can be a 2D or 3D sketch ... even a 3D sketch with the path drawn on one plane (2D) will work.

The Paths start point does NOT have to be coincident to any point of the Profile. However, it does have to be coincident with the plane that the Profile is on.

Can you repost a (smaller) image showing your Feature Manager?


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[Legrand]

Ok... here's the tree:

Sketches are speperate (why I had posted larger pics before). Planes are coincident.

If someone's really bored, they can look at the part here:

http://www.meche.net/images/012965.SLDPRT

I'm just about to the point whee I'm going to do this with a bunch of seperate sketches...

 

[CorBlimeyLimey]

Unfortunately I do not have SW2005, so cannot read that file


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[CADGemini]

I have tried working your file and it seems that the 3D sketch is corrupt in some way. I opened a new part and re-drew the 3D sketch and it worked fine.

I think that it is best to draw your path first then add a pierce relationship to the 3D sketch. It is much more stable than adding a coincident relationship.

Also I would try to add better contraints to your 3D sketch. There may have been something a little out of alignment causing the sketch to fail.

I hope this helps.


Best Regards,
Jon

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[SBaugh]

If you can't run a check sketch for feature then the sketch is corrupted. Try remaking the sketch.

Check sketch for feature is located under tools\Sketch tools\

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

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[SBaugh]

Found something else... if you can't make this 3dsketch into a composite curve (which I bet you can't) You get the error "the sketch has disjoint segments and is not suitable for composite curve creation" then the 3d sketch is broken and that maybe another reason why the sketch will not be used in the Sweep feature.

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
faq559-716 - SW Fora Users

 

[Legrand]

Oh My good glory.....
OK then... somehow, as you've found out, the sketch was "corrupt" (or disjoint, as SW loves to put it). I have never used the "repair sketch" funcion, and don't do much 3D sketching like this at all, but I think I'll remember this one!

I tried to create a composite curve, and, as you said, it errored on me with "disjoint sketch". I did the "repair in the sketch tools, and it's working!

Woot!

Thanks a million guys, sorry this one was so much greif.

Scott