[pixburghenat]

Here's a jpg using a helix. This is 2 that were joined using the composite curve command then a sweep cut.
The second side was mirrored.

The helix command seems to have been improved since the 2007 version.
In 2007, I could only get the same results using a wrap feature.


pix

[JerryFlyGuy]

That could be, or it might just be some different [tiny] detail which made it work this time. 08' also has a 'sweep a solid' ability. I haven't had the need for it but.. it's kinda neat regardless..

[pixburghenat]

I'll have to look for the sweep a solid feature.
This one was a sketch, drawn the same way in both versions in every respect.


I'll have a look at both again and see if there was anything different and try the solid cut. The solid cut would be more what I want anyway, I can use it to mimic an endmill.


pix

[pixburghenat]

The sweep with a body works well, not great, it has a few bugs.

If anyone gets unexpected results, I've found that by sketching in line with the direction of the cut gives the best results. when the sketch is perpendicular to the sweep path, the goofyness shows up.

Also, the composite curve isn't a valid path.


pix

[JerryFlyGuy]

Also, the composite curve isn't a valid path.


pix

I've found that making surfaces and then knitting them, and using an intersection curve on the face of the solid generally is more robust than the composite curve..
FWIW

[pixburghenat]

I'm going to use all surfaces with my next attempt at finding a way to model this helix that models the actual part that I had already made.

My orginial method used the helix in 2007, didn't work well at all, the gap narrowed as the cut sweep through the surface. I then used a wrap feature. It worked just fine to create the shape but when the fillets were added, there were some small compromises necessary to let solidworks add the fillets.

Along comes 2008, helix feature works better and can use a solid body model as a cutting tool. Perfect, just what was needed! It looked like this would do the job, it does but with limitations. Like you can't use a composite curve for the sweep path, huh? So I read the help file, 'composite curves are for connecting curves, edges, and sketches for use with lofts and sweeps'. I've used this command many times when creating an overlap on clamshell type models where a top and bottom half come together to made a nice seam, like where a TV remote is joined. The command creates a path for the sweep to follow instead of using edges, much more robust and useful because the sweep path may not be planar.

Again, this all started with the instrument I was making, I had only drawings from an earlier design that were done in Pro E. I redesigned and made the entire device using Solidworks and was messing around with the 4th axis in Camworks. I found out I only have a rotary license for Camworks on the 4th axis, but I had a Mill/Turn license. I had to model the feature anyway, so began the challange. To make a long story short, I modeled using a wrap feature, programmed the 4 axis using G code, got the part cut, finished device, client demonstrated device at a medical symposium, client was happy, supplied client with the models and drawings, and I moved onto the next job.

I haven't gone back and tried this in Camworks yet, I've been fooling around with the model whenever I get time.

I did get the sweep to cut both helix paths, but I had to add the same solid body to the second path so the second cutting tool would be tangent to cut body. It was a work around, it had a few bugs too, but at least it was closer to doing what I expected. As I posted earlier, your results may differ if the cutting tool body is sketched on a different plane, even tho it's a revolved body, Solidworks isn't using the entire body to make the cut. It seems to be using a algorithm based upon the sketch plane and where said sketch intersects the cut body to derive the cut path. I thought I had it once, preview showed the path, everything looked good, click OK, Soildworks said ERROR can't do it, ahhh THAT makes sence! LOL!


I hope I didn't make too many spelling and grammer errors....


I'll post a photo of the completed device. I have to find it....


Thanks for reading,


Scott

[pixburghenat]

Here's a photo of the semi finished project.

The items in the coin envelope are 20 fiberoptic strands 1 meter long.
They had to be oriented and mated to a delrin connector then
encased in PTE tubing and potted with an approved resin that holds up to autoclaving.

[pixburghenat]

I think I got it to work using comp curve and helix.

I added a short extrude and redid the sweep cut from that point.
It seems to work fine.

I had tried this in 2007 and it didn't work so I thought I'd try it again.

The clue came when I started using surfaces, I sweep the arc along the helix path and it was narrowed again, so I added the extrude then sweep and everything lined up.


Now I'll finish the part and compare in GeoMagic.

Thanks,


Scott