Pattern a loft?

[PhilipFry]

Is it possible to make a circular pattern of a loft? I'm trying to pattern a bracket I made with the loft function around a cylinder, but I get the following error:

"Unable to create contour geometry. Please check the loft section."

What part of the loft section am I suppose to check?

 

[TheTick]

You could create the loft as a surface and pattern the surfaces...

"Great ideas need landing gear as well as wings."--C. D. Jackson

http://www.EsoxRepublic.com

 

[CorBlimeyLimey]

Is your loft a separate body in a multi-body part? If not can you make it into one & then pattern the body?

from Barrie, Ontario.

I love defenseless animals, especially in a good gravy.
faq559-863

 

[PhilipFry]

Limey,

I'm not totally familiar with your terminology. Are you talking about an assembly as opposed to a part, or a part with seperate bodies?

I "grew up" with SW 2001, where you couldn't have seperate bodies in a part, so SW 2003 was a big change for me. How do I go about seperating a loft, whose shape is dependant on the other two bodies?

 

[CorBlimeyLimey]

I'm talking about a part with separate bodies.

I assume you are creating a loft from a sketch shape on the circumfernce of a cylinder and are lofting to another sketch shape a distance away from the cylinder.
To create your loft, select the two sketches, & in the options section of the loft dialogue box, deselect the "Merge" option. That will create the separate body. Then simply do a circular pattern using the cylinder axis & the lofted body.

from Barrie, Ontario.

I love defenseless animals, especially in a good gravy.
faq559-863

 

[CorBlimeyLimey]

Like this?

from Barrie, Ontario.

I love defenseless animals, especially in a good gravy.
faq559-863

 

[PhilipFry]

Yes, that's the idea at least.

Hears another question. How do the parent/child relationships work when you are dealing with multiple bodies. When I first tried seperating the loft from the other bodies, I kept getting 1 of 2 error messages:

"blah blah blah...zero geometry"
or
"loft failed"

I got it to work, but I'm not sure how or why.

 

[CorBlimeyLimey]

I don't know why you are getting either of those errrors.

How are you creating your sketches, especially the one on the cylinder. I created mine within a 3D sketch using the edges of a rectangular hole in the cylinder & a simple elipse drawn on an offset plane.

BTW: I also did the above model without using multi-bodies & without any problems or errors. I just created the loft with Merge selected, then circular-patterned the loft feature.

from Barrie, Ontario.

I love defenseless animals, especially in a good gravy.
faq559-863

 

[JNR]

Is the error message ....zero THICKNESS geometry...? Maybe you need some guide curves? Example: Imagine a shape consisting of two coaxial cones, point to point. Though they are theoretically continguous, they cannot exist in SW (or any other solid modeller I am aware of) as part of the SAME body. The thickness at the "point" in the middle of the body is zero and the math does not like this... "Can not compute, earthling!" If your loft is getting confused where the start locations of the two (or more) profile curves are and is trying to twist in the middle it can result in this condition. Using guide curves will fix this. Another problem can occur (with sweeps, also) where the path and profile are such that the surface is trying to go back over itself again - it does not like this either. You can sometimes fix this by finding the point where this occurs (most often an inflexion - reverse curvature - in the path) and breaking the surface sweep or loft into parts either side of this location. I had one of these yesterday sweeping a head profile along a crash test trajectory. There was a very small section of curve at the begining that had a slight inflexion. The initial result was quite spectacular, but not even remotely what I wanted. It was difficult to imagine how the simple path and profile could product such a contorted goober. .........My eye balls did however eventually settle back in their sockets.

John Richards Sr. Mech. Engr.
Rockwell Collins Flight Dynamics

A hobbit's lifestyle sounds rather pleasant...... it's the hairy feet that turn me off.

 

[PhilipFry]

Well, the "sketch" on the cylinder isn't exactly a sketch. I drew the basic profile on a reference plane going through the center of the cylinder and projected a split line onto the surface.

There should be no twists...and don't see any in the preview either. I am using a curve/straight line as a guide.

 

[CorBlimeyLimey]

That's probably why you were having a problem. Try creating a true sketch on the cylinder. Also make sure when extruding the loft, that you are not getting the "zero geometry" error by having a wall thicknes meeting or "Merging" only at the edges of the cylinder aperture/split. Although if you are using multi-bodies that shouldn't matter.

from Barrie, Ontario.

For Sale: Parachute. Only used once, never opened, small stain
faq559-863

 

[APPENG]

Just out of curiosuty have you tried using the geometry pattern option? If so what were the results..



Regards,
Jon
jgbena@yahoo.com