Revolved Loft? 3

[rjmax]

Is it possible to do a revolved loft? Trying to draw a satelite dish with parabolic contours and would like to do a revolve loft to the contours.

 

[Heckler]

Yes, you can revolve a loft. Right from SWx help menu

Select the profiles to loft in the graphics area for Profiles .

Under Centerline Parameters:

Select the centerline sketch in the graphics area for Centerline


Best Regards,

Heckler
Sr. Mechanical Engineer
SW2005 SP 2.0 & Pro/E 2001
Dell Precision 370
P4 3.6 GHz, 1GB RAM
XP Pro SP2.0
NIVIDA Quadro FX 1400
o
_`\(,_
(_)/ (_)

"There is no trouble so great or grave that cannot be much diminished by a nice cup of tea" Bernard-Paul Heroux

 

[Heckler]

I need to add one other item, you will need two profiles to complete the loft. The other week I made a spring. I created a composite curve out of three helix and had a two profiles then made a loft. But now in 2006 we have a varable pitch helix....

Best Regards,

Heckler
Sr. Mechanical Engineer
SW2005 SP 2.0 & Pro/E 2001
Dell Precision 370
P4 3.6 GHz, 1GB RAM
XP Pro SP2.0
NIVIDA Quadro FX 1400
o
_`\(,_
(_)/ (_)

"There is no trouble so great or grave that cannot be much diminished by a nice cup of tea" Bernard-Paul Heroux

 

[rjmax]

What you described doesn't work for what I am doing. I have one parabolic contour on one plane and another parabolic contour on another. They both share the same axis at the center and I want to revolve around that shared axis and loft the two contours. Any other ideas? What you told me is the centerline is a guide curve for the two contours to follow and I just want to revolve around that centerline not use it as a guide curve.

 

[CADGemini]

rjmax,

Can you share a picture with us so we better understand what you are trying to do?

Have you tried revolving each contour 180° and joining them as one solid body? Or maybe revolve each contour 180° and then loft between the two profiles to connect the two solid bodies into one. I might be unclear of what you are trying to achieve. Without a picture I am guessing.

Best Regards,
Jon

Challenges are what makes life interesting; overcoming them is what makes life meaningful.

Solidworks 2005 SP3.0

 

[CorBlimeyLimey]

Perhaps I am missing something here, but why can't you just do a simple revolve of each, or join both contours using the composite curve feature & then do one revolve?

Perhaps if you post an image (faq559-1100) we can offer the correct advice.


Making the best use of this Forum. faq559-716
How to get answers to your SW questions. faq559-1091
Helpful SW websites every user should be aware of. faq559-520

 

[RocketRonnie]

Sounds like a rotational blend, it's been in Pro/E for years, but I can't find it in SolidWorks.

 

[Arlin]

I am a bit confused by your description. Is this what you are trying to do?

http://img25.echo.cx/my.php?image=parabolaloft6ln.jpg

You say you are creating a parabolic dish, but using 2 parabolas. To create a true parabolic dish, all you would need to do is create ONE parabola and revolve it around its axis.

In my example, I have used to parabolas as you described and used an eliptical guide curve.

 

[sreid]

I no nothing about Solidworks but a NURBS surface can exactly specify a conic surface.

 

[rjmax]

Arlin, what you have there is exactly what I am trying to do. Any advice?

 

[Arlin]

rjmax,

What I did was create the two parabolas on perpendicular planes.
Create the eliptical guide curve that intersects the parabolas.
Create a Loft with the two parabolas, selecting the elipse as a guide curve.
This will give you 1/4 of your dish.
Now use the mirror bodies command to create the other 3 quadrants.

 

[rjmax]

Arlin,

That did it! Thanks a ton!

 

[CorBlimeyLimey]

Good call Arlin ... How long have you been psychic?


Making the best use of this Forum. faq559-716
How to get answers to your SW questions. faq559-1091
Helpful SW websites every user should be aware of. faq559-520