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| An example of a part requiring a thread |
That meant, eventually, I was going to be faced with making a thread. What made me nervous was how to I make the thread work? Especially since I typically deal in machine threads? Machine threads can get pretty fine.
First, I want to get the acknowledgements out of the way. I didn't come up with these ideas on my own. I started by watching the following videos, and adapted them to fit my needs.
The first is from KETIV Technologies, and the second, from 3D Printing Nerd. Those videos are certainly worth taking a look. But I did need to tweak their procedure to get the result I needed.
So here's a quick rundown of the procedure I used, with a couple of changes I made to make it work for me.
I'll be using Fusion 360 for this example. I've found it gives me the best results, but I'm sure other CAD tools can perform similar functions.
Here we go!
Thread Reliefs are Not a Relief
First of all the part I work with often have thread reliefs modeled in. I found out the hard way that these can sometimes interfere with the thread lead in. I've had the best luck deleting them and making sure the thread starts right at the end of the desired starting point.
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| The thread relief has been deleted. Click image to enlarge |
Tune up the Virtual Tap and Die Set
After deleting the reliefs, the modeled thread needs to be added. This may be done by editing an existing thread, or creating a new one if a thread feature doesn't exist. Fusion 360 has a check box that models the thread, Other programs have different methods of adding the thread.
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| The modeled thread and dialog box. Click to enlarge image. |
Practice Your Scales
Now comes my challenge and the solution I found for that challenge. I needed to scale the thread to increase the clearance between the mating thread so it will thread smoothly. But I can't scale the entire part, because the rest of the geometry needs remain the same size.
So I split the part into two different solids. In this case, I used an extruded surface as my splitting surface. The diameter of the surface is only slightly smaller than the minor diameter of the thread.
Remember the goal is to scale the thread, not anything else!
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| An example of the surface that becomes the cutting tool. Click image to enlarge |
Now the solid containing the thread can be scaled. For the parts I work with, I only scale radially. The thickness is left alone.
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| Scaling the solid that contains the thread. Note the use of Non-Uniform Threading Click image to enlarge |
As far as the amount to scale, I've found that it varies. I've done between 0.5 and about 5 percent. With larger percentages working for smaller threads. However, I'm still working on the guidelines, so I wouldn't consider these numbers absolutes.
Check the Thread Clearance
As a final check, I compare the part to it's mating thread, assuming I have it, and if I have what looks like a good clearance, I roll with it.
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| Comparing the mating threads to eyeball the clearance. Click image to enlarge |
I know it's not very scientific, but so far, it's been effective.
Glue it all Together with the Combine Command
For my final step, I combine the solids back into one. Now the part is ready to be exported as an STL file, and imported into your slicer.
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| Combining the two solids back into one. Click image to enlarge |
Speaking of slicers, I use Simplify3D at work. And what I've also found works best is to remove any supports that are automatically generated inside the thread. I've found they aren't needed, it's just that Simplify3D thinks they are.
And thus far, these guidelines have worked well for me. Feel free to take them and give them a try, and modify them as you see fit!
Good luck! I hope this is helpful! I hope you can take these ideas and use them as seeds to develop your own.
And please share your tricks with others!