×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Helix to follow a path
5

Helix to follow a path

Helix to follow a path

(OP)
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.

RE: Helix to follow a path

If it simply a circle, as your steps would indicate, you can use a revolve feature or a swept feature. The revolve would be easiest.

Jeff Mirisola, CSWP
http://designsmarter.typepad.com/jeffs_blog

RE: Helix to follow a path

3
To do that involves two steps;

1) Create a Swept Surface using a straight line as the profile, a circle as the path and using the Twist along path option. Specify 360° x number of turns required. This will create a surface which spirals around the circular path.

2) Create a Swept Boss/Base using a circle as the profile and one edge of the swept surface as the path. This will create the "Garter Spring". You then need to delete the surface body created in step one to finish the model.

cheers

RE: Helix to follow a path

2
Like this.

RE: Helix to follow a path

Exactly like that. smile

cheers

RE: Helix to follow a path

(OP)
Thank you handleman for the download, but I can not open it because our IT department still has not upgraded us and I am still stuck with 2006.  Thank you also CorBlimeyLimey, I am still trying to get your suggestion to work, because I have never used these items before.  I created the line and a circle on the front plane and I can not get swept in surfaces to un-gray so I can use it.  I will keep on working on it and maybe I will figure it out soon.

RE: Helix to follow a path

(OP)
Thanks Scott, I have already seen this file and in fact I use the fake thread allot in my models.  I am reading everything in help on swept surface and I hope to have it figured out shortly, but right now it is the first time I have worked with it and it is not starting, so to speak.  

RE: Helix to follow a path

(OP)
Well, I finally got it working, some what.  I have the path circle at .750 and the line at .053 and it is centered on the circle.  I got it to go up to 66 turns and then it bombs out on me saying "Smooth path is needed for sweep to twist."  I don't understand why I am getting this message on 67 and more turns.  It looks like 90 to 110 is probably were the number of turns should be.  Anyone have any insight on this?  Thank you again for all of the help.

RE: Helix to follow a path

You don't necessarily want the line to be centered on the circle.  If you do that you will create a double helix.  Just have one end of the line pierced by the circle.  The other end will trace your helix.

RE: Helix to follow a path

I think SW is having trouble making the sweep join back up to itself when it goes all the way around the circle.  If you will make the tiniest break in the path circle (1 degree angle or so) then SW won't try to join the sweep back up to itself and the feature should succeed.  However, I believe the number of twists is limited to 100, so you're not going to be able to get your 110 turns without doing some sort of circular patterning.

Also, you know you are going to absolutely slaughter your performance, right?

RE: Helix to follow a path

(OP)
Thanks handleman, I currently have it centered and it looks great up to 66 turns and then from 67 turns on I blow out with that message.  I did try the one end piercing the circle and I got the same results, except that the max number of turns is now 65 instead of 66.  and yes I got the exact same message.

RE: Helix to follow a path

(OP)
Thanks CorBlemeyLimey, but it says it still can not recognize the version.  I am using SW Office 2006 sp4.1.  It looks good except for it needs more turns.  

RE: Helix to follow a path

As I said before, SW is having trouble joining the ends of the sweep together.  I can't imagine the level of math required to make the sweep meet together smoothly, and I'm sure the problem probably has to do with something being rounded off somewhere.  You are going to have to make a break in the circle you are using for the sweep path.  And even then you will be limited to 100 turns max.

RE: Helix to follow a path

ponder If it cant recognize the version (and I assume can't be opened) how can you tell if it needs more turns?

BTW, I kept the turns low to reduce file size. The idea was only to show how it can be done.

cheers

RE: Helix to follow a path

(OP)
Thanks guys for the help, I think I will just play with it and see if I can get those 100 turns.  As for file size that is no problem because the server is huge and there is plenty of RAM on this machine.

RE: Helix to follow a path

CBL was trying to keep file size smaller to reduce upload/download time, not for storage space or performance opening the file.  

You're not going to be able to increase your number of turns until you break the main path circle.  If you make the main path circle (the one that's 0.75 diameter) into a half-circle you can make as many turns (up to 100) as you want on the half-circle, then create a circular pattern of that surface body to form the complete circle.  It doesn't matter that the two surface bodies are not joined into a single surface body.  The final sweep that you do along the path will be a continuous solid body.  I just generated a garter spring with 200 turns.  As I said before, however, performance takes a huge hit.  The model takes 80s to rebuild on my dual Xeon, 3GB, QuadroFX 3400 box.

RE: Helix to follow a path

(OP)
Thanks, I'l give it a try.

RE: Helix to follow a path

(OP)
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.

RE: Helix to follow a path

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.

RE: Helix to follow a path

(OP)
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.

RE: Helix to follow a path

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.

RE: Helix to follow a path

(OP)
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.

RE: Helix to follow a path

(OP)
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.

RE: Helix to follow a path

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

Rodrigo

www.morrisonpump.com

RE: Helix to follow a path

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 pc2
www.scottjbaugh.com
"If it's not broke, Don't fix it!"
FAQ731-376: Eng-Tips.com Forum Policies

RE: Helix to follow a path

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.

RE: Helix to follow a path

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...

RE: Helix to follow a path

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 pc2
www.scottjbaugh.com
"If it's not broke, Don't fix it!"
FAQ731-376: Eng-Tips.com Forum Policies

RE: Helix to follow a path

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.

RE: Helix to follow a path

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 pc2
www.scottjbaugh.com
"If it's not broke, Don't fix it!"
FAQ731-376: Eng-Tips.com Forum Policies

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources