Helix to follow a path 5

[quest4k]

I am trying to make a Garter Spring, which is a circular spring, to put it simply. I made a primary circle on the front plane and then I made the helix profile circle on the right plane and then I pierce the pierced the primary circle with the helix profile circle and I was fully constrained. Then I opened up the helix and do you know what it did? It shot straight out in a straight line instead of following the path of the primary circle. Is there any way to get the helix to follow the circle path? Thank you in advance for any assistance rendered.

 

[quest4k]

Well, I did try it and it is almost working correctly, but when you have 65 or more turns body delete does not work correctly, it deletes the half of the profile you are working on. Am I missing something here? Thanks. again for everything.

 

[handleman]

OK, here are the steps:

1. Draw 0.75" diameter semicircle on Top plane
2. Draw vertical line on Front plane, one end pierced by semicircle
3. Insert->Surface->Sweep, choose profile and path, and twist along path 100 times
4. Insert->Reference Geometry->Axis defined by intersection of Right and Front planes
5. Choose inserted axis and surface body, Insert->Pattern/Mirror->Circular Pattern, 2 instances, equal spacing, 360 degrees
6. Insert->3D Sketch, select half of the full helix, convert entities. Select the other half, convert entities.
7. Delete both surface bodies
8. Insert->Reference Geometry->Plane, Normal To Curve, check Set Origin On Curve
9. Sketch wire diameter circle on inserted plane, center of circle coincident with helix sketch.
10. Sweep wire diameter sketch along 3D sketch.

 

[quest4k]

Thanks for the info, but me and this software just don't like each other. I got as far as the circular pattern and it would not recognize the surface body and so with that now shot down, I am taking the better part of valor and giving up. I have wasted enough time on this part and it is just going to have to do and if someone does not like it let them make it. With that all said, I am going home, so have a great night.

 

[handleman]

Sorry you're having such rotten luck with this part. This may be a difference between 2006 and 2007. Just as a last-ditch check, you are using the "Bodies to Pattern" part of the circular pattern, right? If "Features to Pattern" is active then it won't pick that body.

 

[quest4k]

Thanks handleman, I tried it one last time and this time I click one the surface bady about 20 times and one of them finally caught and so I continued and everything was going well, till I got to the last line and I tried to sweep the wire diameter. The sweep recognizes the profile, but it won't recognize the 3D sketch.

 

[quest4k]

Success, finally. I went back to the two halves and pulled the edges into a 3D Sketch and used the last half of these instructions and it worked with 90 turns per half. I found out what was making my mirrored surface not work, it was that little line on the front plane. So thnaks again for all of the help.

 

[MPCLima]

save your work before attempting to make a helix. sometimes SW chokes up. Good luck

Rodrigo

http://www.morrisonpump.com

 

[SBaugh]

Well I found an example here at work like what wanted above, but its tapered. You can see in the part how it was made, maybe this will help and lessen the amount of features and steps.

But this file is in SW07. You can install SW07 next to your SW06, just place it in a different folder then what is given to you by default. (C:\Programs Files\Solidworks07\)

http://www.4shared.com/dir/3630673/6ec9121c/Eng-Tips.html

You would have to modify it to fit your design and requirements, but even from the image file that I provided you can see that's possible to do it a far less steps.

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

"If it's not broke, Don't fix it!"
faq731-376

 

[handleman]

Scott,

I really don't think it's possible to do with fewer steps than were listed above. Ideally the circular pattern steps should be eliminated. However, SolidWorks can't seem to calculate the continuous surface body when it's swept with a twist more than 67 turns, and 100 turns is the limit for a single sweep even if you do put a gap in the circular path.

 

[SBaugh]

You can change your Helix or multiple helixes to a Composite curve and use that for your path. Seems like the best approach to me.

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

"If it's not broke, Don't fix it!"
faq731-376

 

[handleman]

So, the only change you are suggesting is to use a composite curve rather than Convert Entities in the 3D sketch? Sorry to be a pain, I'm trying to learn myself the best way to do this. I'm pretty close to my depth limit on this swoopy stuff...

 

[SBaugh]

Not just the only thing... I looked up an image of a garter spring and it shows the spring to get more compressed towards one end of spring. This where I would make a couple of helixes or if you follow the model i uploaded to that site. You may have to make multiple sweeps to get the compression your looking for. You could use a 3Dsketch but then you should convert that to a composite curve. So you have a single path versus multiple paths.

I will see what I can come with in SW06... working on it now, its close but its twisting.

Thanks,

Scott Baugh, CSWP

http://www.scottjbaugh.com

"If it's not broke, Don't fix it!"
faq731-376

 

[handleman]

Oh, so you're also talking about modeling the tapered portion that's inserted into the other end to physically join the actual garter spring into a circle? I was just ignoring that and creating a completely continuous toroidial helix. Adding the taper on the end would certainly require the methodology you used in the sample you posted. Since the continuous toroidial helix didn't have a taper I just skipped the intersection curve portion and created the sweep path directly from the edge of the twisted, swept surface. When I created the 3D sketch and converted entities on the edges of the surface bodies, it created two 3D splines that were continuous enough to be interpreted as a single sweep path by the sweep function.

 

[SBaugh]

http://www.4shared.com/dir/3630673/6ec9121c/Eng-Tips.html

There you will find a SW06 file. It took more work then I expected, but it looks more like the garter spring I saw. However the where each spring connects the angle is wrong... I don't have a lot of time to put this together correctly, but you can see from the model that it can be done... I think its going to be easier in SW07 or even 08 when it comes out.

I hope this helps explain it better I didn't use a Composite curve I made each one separate. I am sure with more time and patience one could make this much better.

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

"If it's not broke, Don't fix it!"
faq731-376