This topic comes up over and over again, so I thought that IÆd put together some of the more popular ways to create a thread in a part environment along with some statistics and reasoning as to why one method would be preferred over another. It should be noted that this may not be a complete list of threading methods, since in this case there is more than one way to thread a cat.
Before you decide to cut threads into your part, a design decision must be made which determines the relative value of modeling the threads. Thread features are often very resource intensive at the part level, and that issue only magnifies when multiple parts are inserted into an assembly. The best policy, depending upon design intent, is to avoid modeling threads in SolidWorks if at all possible. Having said that, below is a list of six ways to model threads (same process for both internal and external threads) in order of increasing complexity of operations:
I. No threads. This is the baseline from which the other numbers have been extracted. Imagine a simple socket-head cap screw shape without threads. # of features = 4. Rebuild time = 0.00-0.02 sec.
II. Cosmetic Threads. Go to Insert/Annotations/ Cosmetic Threads. This paints a visual representation of threads onto your feature. It also imports a thread callout into your drawing. This method does not add any features to your model, and it does not increase rebuild time. It is somewhat parametric as it will partially update with design changes. The disadvantages are that it doesnÆt look very realistic, behaves quirky sometimes, and doesnÆt show up in model rendering. # of features = 4. Rebuild time = 0.00-0.02 sec.
III. Simple Swept Profile. Draw a line following the temporary axis of your feature. Draw your thread profile. Do a Swept Cut, and choose Twist Along Path. Input the number of turns required. This is a very quick and easy way to cut threads into your feature. It is partially dynamic depending upon your sketch relations. # of features = 7. Rebuild time = 0.06-0.09 sec.
IV. Revolved Threads. Draw your thread profile. Do a Revolved Cut around your temporary axis. Do a linear pattern of your cuts. Again, this is a quick and easy way to model threads. The disadvantage is that it is not an actual thread since the cut is revolved and not swept. This method serves to get the point across without being too resource intensive. # of features = 7. Rebuild time = 0.09 sec.
V. Helix Method. Draw a helix that wraps around your feature. Draw your thread profile. Do a Swept Cut of your profile following your helix. This is a very realistic method for creating threads, as you can control the pitch, height, starting angle, etc. of your helix in a simple property manager. The major disadvantage is that helixes are notoriously resource intensive, and it is not dynamic. The amount of resource that swept cuts following a helix command depends upon many factors including the pitch and how/where the cut starts. # of features = 8. As far as rebuild time goes, I got significantly variable results in the range of 0.20 to 45.34 sec depending on how I constructed the cut. With the cut starting 180¦ from the helix start point, I was able to reproducibly get 0.20 sec rebuilds.
VI. Swept Surface. Draw a line following your temporary axis. Draw a line perpendicular with that line (in a separate sketch) that is collinear with the top or bottom of your feature (or wherever you want your cut to start). Pick Swept Surface and sweep the second line around the first with a Twist Along Path option. Match the parameters to your thread pitch. Convert the edge of this surface into a 3D sketch. This should essentially be the same as a helix. Draw your thread profile. Do a Swept Cut that follows the 3D sketch. Although this method seems like it is overly complicated at first, it has the benefit of being completely parametrically driven depending upon your sketch relations. It will update your cuts to your model changes. The major disadvantage is that it is a resource hog. # of features = 10. Rebuild time = 18.33-19.86 sec.
If threading is something that you have to do very often then I would suggest creating Design Features and reusing them. If you use standard threads you can even create ôTapsö and ôDiesö that you can position in your parts and use the Combine Feature to remove the material where your threads should go. All of these design methods depend on the environment that you work in and what the intent of the project is.
If this is something that you run into often I would suggest that you submit an enhancement request to SolidWorks and talk to your VAR about the necessity of a thread-creation utility that works similar to the Hole-Wizard. Then waitàpatientlyà
