Drawing a tapered screw with true helical threads

[Izmar]

Hi,

I'm trying to use Solidworks to draw 3D models of orthodontic miniscrews. I found some tutorials online and could successfully draw cylindrical screws with true helical threads (by using the swept boss feature over a helical curve), but I could not draw "tapered" screws because when I use the sweep cut or boss feature the thread size changes as it follows the helix of the curve (it is small at the beginning and gets larger at the end).
I wonder if there is a way to make the thread follow the surface of the screw in addition of the helix so that it has a constant size.
Otherwise, is it possible to "taper" a previously drawn cylindrical screw with threads?

Thanks

 

[BoomerSooner7]

Izmar,

Use the taper helix option when creating the helix. Make sure the taper angle and base circle dimensions match on both the helix and the geometry you are cutting the threads into. You will follow the same procedure as cutting cylindrical threads. Hope this helps.

BS7

 

[Izmar]

I did the same thing you mentioned but it seems the cut follows the helix in 2D not in 3D so the thread becomes larger the closer you get to the taper!

any other thoughts?

 

[rollupswx]

I did the same thing you mentioned...

Can you attach what you have so far and indicate SWx version?

 

[Izmar]

I am using SW 2008 SP0.0

My problem is in the threads. They do not look like the design I want and their size is not consistent all over the surface.

Here are the screw I drew and the screw I am trying to draw.

http://img404.imageshack.us/my.php?image=screw1bj9.jpg

http://solutions.3m.com/3MContentRe...6E48B1800BAE180A88EBDDE34ECA0&version=current

 

[ctopher]

If you don't need the actual thread (most people don't), just draw a thd profile and revolve it. The helix will use up more RAM.

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 06/08
ctopher's home (updated Jul 13, 2008)
ctopher's blog

 

[CorBlimeyLimey]

Experiment with combinations of the options of the sweep.
Try Follow Path and All Faces.

 

[BoomerSooner7]

Izmar,

I've attached a part in SW2008. I think this might be what you're looking for.

BS7

 

[uGlay]

Are you going to have this screw manufactured?

SW2008 Office Pro SP3.1
Intel Core 2 Duo CPU
2.2GHz, 2.00GB RAM
QuadroFX 3700
SpacePilot/SpaceNavigator

 

[Theophilus]

Here's one I did a long time ago, but it's a bit of a hack (in v2007 format now). Several things you don't want to do are found in this model (as reference) such as having the radius built into the sweep where the thread meets the screw shaft (but SW wouldn't apply the root radius after sweeping in the version I built this a long time ago). Most new versions will probably add the radius without a problem.

Link:

http://www.industrialdesignhaus.com/internet/Screw-Helical-Hack.SLDPRT

Jeff Mowry

http://www.industrialdesignhaus.com

A people who value security over freedom will soon find they have neither.

 

[Izmar]

CorBlimeyLimey

No, but I will use it in a finite element study.

BoomerSooner7

This is exactly what I am looking for. Thank you very much. How do you make the threads on the tapered and cylindrical parts exactly match? this is what I could not do.

Theophilus

Thanks a lot. I have a question though. How did you make the thread become smaller at the tip of the screw?

Thanks everyone, this was very helpful

 

[BoomerSooner7]

Izmar,

If you look at the feature history I basically made two sets of helix/threads, one on a cylindrical face and one that is tapered and them combined them with the create composite curve. Both of these were created by the "height and pitch" so it was easy to control where the helix ended and that the pitch matched. To match them up you have to end one and start the other at the same angle, which is an option you can select when creating the helix and obviously both have to be in the same direction, i.e. clockwise. When you create the tapered helix the base has to be the same size as the start of the cone and the angle has to be slightly less than the taper angle of the cone. Once you get both helixes created, combine them and then create your thread geometry starting on the larger diameter portion of the thread and create a sweep. Whew! fingers are cramping. If you study how I created it, it will become clear to you.

thx

BS7

 

[ctopher]

I don't know how much help this will be, but a start to help with threads:

http://www.youtube.com/watch?v=b0npqkpJDDI

http://www.youtube.com/watch?v=ELNtBVPjHIQ

http://www.youtube.com/watch?v=xlwaua5n-zw

http://books.google.com/books?id=9b...=book_result&resnum=1&ct=result#PRA1-PA355,M1

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 06/08
ctopher's home (updated Jul 13, 2008)
ctopher's blog

 

[Izmar]

BoomerSooner7 and ctopher

thanks so much... I appreciate your help... I think I know how to do it now