Modeling a Tapered Spring - Sweep resulting in "Topologically Invalid Surface" 1

[cbrf23]

Hi, I'm having trouble modeling this spring.
I can get the desired profile curve, but I cannot get it to complete the sweep - either as a surface or a solid. I need a solid as the end product, but I'm open in how to get there.
Any help would be appreciated, I've attached the file below.

Also, this is my second attempt at this spring. My first attempt I tried my normal approach using the "helix" curve feature with the variable pitch option.
This method using surfaces has given me better results with some parts in the past, so I tried it, but still no luck.

Thanks again!!

 

[SBaugh]

I think its because your using a 3d sketch as your path. I recreated your spring using a series of sketches, 1 surface, 2 helixes, 1 composite curve and a single feature. I did not set equations up, but the sketches I used use the exact dimensions, so you can set mine example up with equations.

Yet another reason why 3D sketching is not a great tool to utilize... I stay away from 3D sketches, due to there instabilities.


Scott Baugh, CSWP
Berry Plastics
Cad Admin\Design Engineer
GEASWUG Greater Evansville Area SWUG Leader

http://www.scottjbaugh.com

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

faq731-376

 

[Eltron]

It looks like your profile diameter is too big. It works if I drop it down to 0.11".

Dan

http://www.eltronresearch.com

Dan's Blog

 

[SBaugh]

Dan,

Is used the same dimensions, including the .138 diameter and it works fine. I believe its the style of the path used. check out my file.

Regards,

Scott Baugh, CSWP
Berry Plastics
Cad Admin\Design Engineer
GEASWUG Greater Evansville Area SWUG Leader

http://www.scottjbaugh.com

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

faq731-376

 

[cbrf23]

Dan, that is perfect. Thank you very much!

Do you happen to know why your modeling technique works and mine did not?
Prior to the file I attached, I had tried this using a single helix (variable pitch) and the same curve for the hook part, joined as a compound path the same way yours is, and that also failed.
I'm just trying to understand why Solidworks likes one path and not another so that I can avoid delays in the future.

Thanks again!

 

[cbrf23]

Help, I'm really confused now!
I took your example and I tried to re-create it because I wanted to learn and I also wanted to re-create it using our file template, and I do not get the same results.
In my model, I cannot get a single sweep feature to follow the entire compound curve path. (file attached)
The only difference from your model is I've set up the equations, but the end dimensions are the same, and I even went back through yours and I'm not seeing what I did wrong.

 

[cbrf23]

I got it to sweep the whole path - turns out it was an issue with selection before creating the sweep feature.
I was selecting the path and profile before creating the sweep, and for some reason the path was coming in as an "edge" which was not the whole path. I simply cleared this and re-selected the compound path and that fixed it.

However, in my model I get an ugly surface that bulges out at each "joint" in the compound path, not smooth like yours.
I checked and the feature options are set the same, so I'm not sure what I did wrong.
Any ideas?

 

[cbrf23]

I figured this one out.
I had to turn off path start and end tangency.

Thanks again Dan, your file was extremely helpful!!