Drawing a tapered screw with true helical threads
Drawing a tapered screw with true helical threads
(OP)
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
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






RE: Drawing a tapered screw with true helical threads
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
RE: Drawing a tapered screw with true helical threads
any other thoughts?
RE: Drawing a tapered screw with true helical threads
RE: Drawing a tapered screw with true helical threads
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.
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RE: Drawing a tapered screw with true helical threads
Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 06/08
ctopher's home (updated Jul 13, 2008)
ctopher's blog
RE: Drawing a tapered screw with true helical threads
Try Follow Path and All Faces.
RE: Drawing a tapered screw with true helical threads
I've attached a part in SW2008. I think this might be what you're looking for.
BS7
RE: Drawing a tapered screw with true helical threads
SW2008 Office Pro SP3.1
Intel Core 2 Duo CPU
2.2GHz, 2.00GB RAM
QuadroFX 3700
SpacePilot/SpaceNavigator
RE: Drawing a tapered screw with true helical threads
Link:
http://www
Jeff Mowry
www.industrialdesignhaus.com
A people who value security over freedom will soon find they have neither.
RE: Drawing a tapered screw with true helical threads
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
RE: Drawing a tapered screw with true helical threads
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
RE: Drawing a tapered screw with true helical threads
http://www.youtube.com/watch?v=b0npqkpJDDI
http://www.youtube.com/watch?v=ELNtBVPjHIQ
http://www.youtube.com/watch?v=xlwaua5n-zw
http:/
Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 06/08
ctopher's home (updated Jul 13, 2008)
ctopher's blog
RE: Drawing a tapered screw with true helical threads
thanks so much... I appreciate your help... I think I know how to do it now