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Posts Tagged ‘threads’

This one was the first ever hands-on session I attended at SolidWorks World. Last year I wasn’t able to get into any of the hands-on sessions, but this year I had the opportunity to pre-register for several of them and it was one of the best things I could’ve ever done. 

This session was presented by Dan Riffell, Projects Coordinator at Eltron Research and Development. Dan is also a very well known contributor in the SolidWorks discussion forums and engineering community. Dan prepared this session because, believe it or not, how to model a thread is an incredibly common question among SolidWorks users, so he wanted to explain a few different ways to do it that may be useful depending on our needs.

First of all, Dan began by pointing out that we usually don’t need to model threads. Unless we need them for an animation, mold creation or a photorealistic image, for instance, most of the time, we can get by with using annotations and don’t really need a physical representation of the thread in the model. We can add a callout in the drawing with information about the thread or use a special kind of annotation known as cosmetic threads (Insert/Annotations/Cosmetic Threads).  

This kind of annotation appears as a feature in the Feature Manager and you can suppress it or delete it if you don’t need it anymore.

He then showed us how to create revolved threads. He sketched a thread profile and revolved it around the temporary axis of the part, creating a cut ( Revolved Cut), then he created a linear pattern using the revolved cut as the feature to pattern and the part’s temporary axis to define the direction.

Notice that this is not a real thread, but only looks like one, and it’s actually the kind of thread that is usually generated for most Toolbox screws.

The next method that Dan demonstrated involved the use of Swept Cut, as you can see in the image. He used the same thread profile sketch as before as the profile for the cut, but this time we had to create an extra sketch to be used as a path. It was a simple sketch of a line that runs along the axis of the part. The option to twist along path is what makes the profile describe a helix as it travels along the path.

The next method is very similar, but he creates a helical surface first and converts its edge into a 3D sketch to use it as a path for the Swept Cut command. This is similar to what Charles Culp did to create the telephone cord, remember? Notice that this time around the path is already describing a helix, so there’s no need to use the option to twist along path.

Another method to create a helical path for the thread is to simply create a helix by using Insert, Curve, Helix/Spiral, as you can see in the following image. By the way, to use this method you have to start by opening a new sketch on the circular face of the part and converting the edge to use it as the base for the helix. A curious fact: I asked Dan if it made any difference what start angle we chose and he said the rebuild time changes with the angle, for some strange reason.

Once you have the helix ready, you can use it as the path for the Swept Cut, and, just as before, there’s no need for the option to twist along the path.

 

What Dan demonstrated next was the coolest part, because he showed us how to create a design library feature to add threads to other similar parts without having to go through the whole process again and again.  First, he opened the Design Library Tab in the Task Pane and dragged the SweptCut1 feature from the Feature Manager tree  to the Design Library’s lower pane. A property manager appeared, as you can see in the image. From this property manager we can choose a folder where to store our new library feature and/or add a tooltip to remind us what this library feature is for.

Once the library feature has been added to the design library, we’ll see it in the lower pane or in whatever folder we placed it and we’ll be able to use it in other parts simply by dragging it from the lower pane and dropping it on the graphics area. In this example, after we drop the library feature, SolidWorks prompts for us to select a placement plane. Other selections will be necessary, as well (an edge, a sketch point and a face). All these reference selections are defined by the relationships that were used in the thread profile sketch. For instance, the thread profile was sketched on the Front Plane, so the Front plane should  be our selection for Placement Plane.  A little display pops up to help us along the proces,s by giving us visual clues of what we’re expected to select. In the image below, for instance, we are expected to select that circular edge we see there.

Once all our references have been selected, the thread is added to the part.

Last but definitely not least, Dan showed us how to model an inner thread, such as the ones in nuts, to match the outer one. We started with the model of a nut and inserted the screw we had been working with before by using Insert, Part.  We located the part as you see it in the image by adding a concentric mate  and a distance mate between both parts.  Remember, this is not an assembly, we inserted a part into a part.

Next, Dan showed us how to use Combine (Insert, Features, Combine) to subtract the screw from the nut, as you can see in the image. The nut is the main body (in green) and the screw is the body to subtract (in blue).

As a result of this operation, SolidWorks will remove or cut away the parts of the nut that overlap the screw, creating the inner thread. Neat!

As I said before, the step by step procedures and files for this and other presentations will be available in March. For now, I hope my little summary may be helpful to somebody.

Thank you, Dan, for this great presentation!