sweep issue on ellipsoid

[finisher]

With reference to the attached file the sweep fails as soon as I add dimensions to the initial ellipse sketch. Why is that? I was able to dimension the sweep path (the line) thus having some but not full control of the aspect ratio of the ellipsoid. How can I fully dimension this solid?

Walter SW 2008 SP 5.0

 

[JMirisola]

Delete the relationships between sketch 2 and 4. Move 4 in front of 2 and dimension it. Create pierce mates between the top and bottom points of the ellipse and sketch 4. Dimension between the horizontal points of the ellipse.
I've seen the issue you're having before, but don't remember the cause. Not sure, either, why my solution works, but it does.

Jeff Mirisola, CSWP, Certified DriveWorks AE
CAD Administrator, Ultimate Survival Technologies
My Blog

 

[finisher]

Jeff, Thanks for your reply. I tried to follow your instructions but still have issues: (1) When I change the dimensions of the profile ellipse the pierce constraints with the guide cuve don't hold; (2)I did place sketch4 (the guide curve) first but then when I did the sweep the order of sketches was automatically restored to the original sequence AND a totally different shape resulted?! File _1 attached is my original and file _2 is my attempt at following your instructions.

Walter SW 08

 

[SBaugh]

Without looking at the file, have you tried doing it as a surface and see if that works? If it does then you can just thicken the surface to a solid.

This is a workaround I sometimes do if I can't get the solid to work. Then I send the problem file into my VAR.

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

"If it's not broke, Don't fix it!"

faq731-376

 

[rstupplebeen]

See attached file and picture. I did a boundary surface from 1 half of the ellipse to the half ellipse perpendicular. I also made a partial ellipse in the third plane to use in the second direction. I hope this helps.

http://files.engineering.com/getfil...5-968b-2f58f5af3869&file=ellipsoid_rob.SLDPRT

http://files.engineering.com/getfil...4888-901d-3cb441644c67&file=Ellipsoid_rob.JPG

Rob Stupplebeen

 

[SBaugh]

Check out this thread - thread559-261983

Might help some.

Cheers,

Scott Baugh, CSWP

http://www.scottjbaugh.com

"If it's not broke, Don't fix it!"

faq731-376

 

[finisher]

Thanks everyone for your inputs. I was finally able to achieve a fully dimensionally controlled ellipsoid using surfaces. I'll keep working on the solids approach.

Rob, I wasn't able to play with your file as alas I am in the SW-08 dark ages! Thanks for the jpeg.

Walter SW 2008

 

[rstupplebeen]

Sorry about the file being in 09. Did you follow what I did? I can not remember if boundary surfaces were new in 08 or 09. If you don't have them use a surface loft instead.

In general surfaces are more powerful or certainly more appropriate for certain situations. If the model does what it needs to do and is not too convoluted then there is no reason to redo it with solids. I hope this helps.

Rob Stupplebeen

 

[laik]

Tried to use the loft? I think it gives a better result than the sweep.

 

[mjcole]

Single Feature no mirror.

Did for Tips&Tricks presentation in 2008 if I have model I can attach but the pictures below show Path& Guide sketch Circle as path and Ellipse as Guide Curve then draw closed Partial Ellipse Dimension the third radius and pierce with guide curve.

In order to select a portion of the multi profile sketch right click while selection is active and Choose Selection Manager shown in image below. Options are
icon1 Closed Loop, highlighted
icon2 Open Loop,
icon3 Group Sel(allows 1by1 selection),
icon4 Region, and icon5 Regular Selection (entire sketches/features)

If you do with 2 Flex Features which is also possible there is a display bug where the Ellipsoid has a line down the second squish or stretch feature along the Sketch plane.

Michael

 

[laik]

Here is a part. Yesterday I could not upload it

 

[finisher]

Rob,

After installing SW10 SP 2.0 at home I opened your surface solution. I find the same oddity as in my solution - i.e., you can change the aspect ratio of the profile ellipse but you have to delete those dimensions or the sweep will fail. This is frustrating me to no end. Not looking for other soutions just an understanding of why this is so.

Walter SW 08 in office, SW10 at home

 

[rstupplebeen]

I dug into this a little farther. In short I do not have an answer but here is my theory and what I did. I believe that the partial ellipses are flipping their direction causing the surface to become twisted. In the end I would call this a bug.

Here is a diary of my failed attempts which might be helpful.
First I tossed pierce, coincident, horizontal and vertical constraints everywhere. The model updated for everything except for the thickness of the ellipsoid. I then extruded the curves into surfaces so I could pick the edges. Still the same error. I then extruded full ellipses and used a split line to cut them. Still same error. I hope this helps.

Rob Stupplebeen

 

[finisher]

I'd like to have the guru's at Solidworks weigh in on this. I have yet to post the question on their forum where they do seem to weigh in on certain issues. They don't seem to do that in this forum for some reason. Thanks, Rob, for looking into it further. I agree - to me it's a bug.

Walter

 

[rstupplebeen]

Post on the surfacing section and link back to here.

Rob Stupplebeen