How to Use the Thread Feature in SOLIDWORKS 2016
TATA Technologies - James Keller | April 4, 2016 | Comment
SOLIDWORKS 2016 introduced the ability to create helical threads on cylindrical faces.
Using the “Thread” feature, users can define the beginning of a thread, specify an offset, set end conditions, specify the size, diameter, pitch and rotation angle and choose various options such as right- or left-handed threading.
Thread types are chosen from a list of custom profile sketches that users can create and store as library features.
In the tutorial video above, we use a lag bolt as an example. We perform a Command Search for Thread and show the command location, which is accessed from the Hole Wizard drop-down menu.
In our example, we select the front edge of the cylindrical face and a preview appears. We’ll leave the default start angle and set an end condition of Blind at three inches.
In this case, we’re using an “Inch Die” type thread because we need to remove material from the bolt like a die would. We can see from the preview that the “Inch Tap” option would be used to create the reverse thread.
If we wanted to add thread material to the model, we could use this option along with the Extrude thread method.
There’s even a default thread option for bottle mouths.
In our example, we use an “Inch Die” type at “0.7500-10.” If the options we needed weren’t available, we could override both the diameter and thread pitch. Additional options let the user change between right- and left-handed threading as well.
Since thread features can be resource-intensive, there are three different preview options to choose from depending on a computer’s capabilities.
Profile options let us mirror, angle and locate a profile. This works basically the same as with weldment profiles.
After accepting the feature to view the new thread, we can see it still needs to extend a little further past the front of the bolt.
We’ll jump back into the feature and check the “Offset” option toward the top, which lets users start the thread at an offset to produce the result we’re looking for in this example. We could also use the sketch point at the front face to define an “Offset Start Location.”
Next, we’ll just update the thread length to make up for the offset.
When users want to save new thread profiles, they will need to save the sketch as a “Library Feature Part” to the location defined under System Options > File Locations > Thread profiles.
Lastly, the Thread feature did NOT replace cosmetic threads. If users find their machine performing slowly using threads, users can still toggle cosmetic threads on or off from Document Properties > Detailing.
To find more tutorial videos like the one shown above, visit myigetit.com.
About the Author
James Keller has over seven years of CAD and instructional design experience, with a primary focus on SOLIDWORKS 3D design software. A strong design background allows him to wear both the hats of Engineer and Designer at once.
- 3D Shape Basics in Fusion 360
- Fusion 360 Sketch Basics
- Running a Parametric Study and Analysis in SOLIDWORKS to Create a Flow Simulation Project
- Calculating External Flow around a Sphere in SOLIDWORKS
- How to Add Heat Sources in SOLIDWORKS
- Working with Macros in SOLIDWORKS Electrical
- Creating Locations in SOLIDWORKS Electrical
- Linking Sketch Blocks in SOLIDWORKS
- Inserting Fluid Subdomains in SOLIDWORKS
- Inserting a Porous Region and Running an Analysis in SOLIDWORKS