Solidworks error sweeping solid along helixes

[cbrf23]

I have to build a part with a cork-screw at one end. I created the path that my cutting tool needs to follow using 3 helixes (helii?). I'll try to explain - see the attached image for further clarity. The first helix is the largest diameter and it is a straight helix. The next helix is tapered - it tapers from the first helix's diameter to a smaller diameter. The last helix is a straight helix from that smaller diameter.

I need to sweep a solid body (must be a solid body, not a profile - I can sweep the profile just fine, its the solid body causing problems) along these helixes.

I can not get this to work. I've tried multiple ways...

First I tried a composite path. Solidworks wouldn't let me choose it - pop up said "path must be fully tangent continuous in solid sweep".

I converted the composite path to a 3-d sketch, trimmed away a little from each helix where they meet, and bridged the gap with a spline which I made curvature continous to each. I tried to sweep along this path. Solidworks let me choose the path, and it looked good when I hit "show preview". I hit the green check, and it processes for a minute before a little box pops up saying "failed to complete" - no further explanation. I'm not sure why, I just know I tried all of the options in the sweep dialog with the same (lack of) results.

Now I tried to sweep each helix individually. I had to create a new solid body (cutting tool) with the same geometry at each helix start point, so I did this using equations to drive my dimensions from the original tool sketch. I sweep the first helix no problem. I can't get the next helix to sweep correctly. It shows a preview that looks good when I choose "show preview". When I hit the green check, it just doesnt do the same thing. The sweep completes, but its all sorts of bad. See the attached images...I can't really explain it.

I'm pretty much out of ideas on this. I'm hoping someone with more solidworks experience (I've only been using this program about 4-5 months) has some insight. I really need to complete this project soon.

I've attached an image which I think shows the problem pretty well.
Unfortunately I can't attach the actual solid I'm working with(confidentiality). I tried creating a test file but couldn't get the exact same results, so I didnt attach it.

 

[cbrf23]

Well, I think I solved the problem.

If I start at the opposite end of the second helix, the sweep completes as expected.

 

[CorBlimeyLimey]

Have you tried using the Variable Pitch helix option?

FYI, plural for helix is helices.

 

[kellnerp]

Sweeps and helices have always been problematic. The helix doesn't have a clearly defined start and stop like a spline.

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[cbrf23]

Hi CorBlimeyLimey, I was unaware of a variable pitch Helix option. I will look into this. Also, thank you for the clarification on Helices.

 

[cbrf23]

Well, the vairable pitch helix is an awesome tool that I didn't know about previously, so thats the good. The bad is that it doesnt create a "tangent continuous" curve, because I get the same error message I got while trying to use the compound curve I created from individual helices.

The solid sweep feature seems week in comparison to the profile sweep. I can't get the thing to do what I want, which is to hold the cutting solid flat and sweep it around the tapered helix....Instead, it keeps trying to rotate the solid to match the helix angle. I tried direction vector and minimum twist, both failed to complete.

Maybe I expect too much out of this program, but I have a very hard time believing that this is not possible...

 

[cbrf23]

Attached an image illustrating the issue I'm having with the tapered helix.

 

[mncad]

Under the Orientation/twist type, select the Keep Normal Constant, I believe this may help you out.

mncad

 

[mncad]

Hi cbrf,

Attached is a quick model I made, I think it takes care of the issues you were having but I'm not sure. I hope you have alot of computer for creating this model....

mncad

 

[cbrf23]

mncad, thank you for spending the time on that. I will try keep normal constant. I thought I had tried that before and just got a generic "sweep failed to complete" error, but I will try it again because it definitely did what I was looking for on your model.

On a side note, I think its funny, because the keep normal constant seems to have very different application/results in the profile sweep context.

 

[rbpmc]

I'm not sure if this applies or not, but I had a similar situation where I needed to create a very simple sweep of a tapered wire with a bend in it. I struggled for 3 hours with this simple sweep using a guide curve to control the taper diameter. I tried every conceivable option in the feature manager. The problem I was having is that I was sweeping from the larger profile along the guide curve that controlled a smaller profile. When I switched and swept from a smaller profile to the larger guide curve controlled profile it worked as expected. I think it was a case where the math just kept tripping over itself. I don't know if there is any relevance but try sweeping from the smaller end of your taper to the larger end.

 

[cbrf23]

Well, after mucking around with it trying to come from different ends of the helixes and trying different combinations of which helix to sweep first, and using keep normal constant, this is the best I could get. Which is obviously no good. I just dont understand why it does this. In the preview, it looks good all the way up to the end of the sweep, then it just gets all jittery.

 

[mncad]

Hi cbrf,

Sorry I can't help anymore. On occasion I get the same kind of surfaces out of the solid sweep cut. The only fix I have found is to make slight changes to the profile or path and sometimes it works. Obviously if your profile and path can't be changed there's not much that can be done. If you can, you should submit that file to solidworks and at least get an SPR started for it. I had a similar SPR a couple of years ago.

mncad

 

[rbpmc]

Another quick thought. Try removing the radii from the profile sketch and add them after the fact on the solid. Maybe it's too complex.