Making Custom Threads

david_winslow625

I'm working on a project where I'm attempting to completely print all hinges. If successful, it'll save me about $100 in hardware.

In my first attempt, printing the male and female parts resulted in pieces cracking when I tried to screw them together, because I had zero clearance between the male and female threads. After watching some tutorials, people suggested scaling the female part by 1.05 in the x and y axis, which provides necessary clearance. This has worked well, the parts screw together smoothly.

Scaling the parts has unintended consequences - ex the outer diameter of the female part also scales. I'm able to manually correct this, but it's more work than I'd like, and made me have to duplicate some sketches.

Here's a link to the OnShape project. In particular, working on the "Tray Sleeve" part

1. Is there a better way to create threads, especially when working with male and female parts?
2. Any suggestions for my creation methods?

Thanks for your help!

robert_scott_jr_

Hey David. Amateur here. I tried Move Face on the female threads, applying the feature to all three faces of the thread. I applied .008" which may be too much. You could probably make a better decision based on how tight you feel the fit is now. If you turn on the sectional view as you apply the feature you can see the result. Perhaps this will work for you. - Scotty

alnis

Here's how I would approach it:
https://cad.onshape.com/documents/3bf5cef509079e4c2fc89b47/w/4bb103895237d2a913234554/e/1658664dc9586dc4327d7894

The overall process:

1. Model new cylinder where you want a screw thread
2. Use the ThreadCreator FeatureScript to add threads to the cylinder
3. Pattern the threaded cylinder parts
4. Use a boolean to cut the threaded hole out of the part with an offset and "all faces" checked -- different thread types in the ThreadCreator FS will allow larger or smaller offsets

There might be a better way, but this is what I typically do.

Screenshot showing threads with clearance:


I hope your project goes well!

michael_mcclain

I've done this type of operation many times for 3D printed parts and I would use a Move Face command on the thread faces to offset them by my variable for tolerancing. (I use Move Face all the time for finish tolerances and connect them to variables in my feature tree)

Dont forget to try the Create Selection option from the right-click menu. Set it to pocket for internal holes or protrusion for external threads.

Argo

alnis Posts: 390 EDU

August 2020

Found this thread when looking for advice on 3D printing threads.
Although there are probably a number of way to approach this - Alnis thank you for posting the boolean offset-all approach. This has worked great for me!

For a starting point for anyone else going down this path:

• Male thread: M9 x 2.5
  
• Female boolean: 0.1mm offset
• Print res: 0.12mm Z, 0.4mm nozzle
• Material: PETG
• Supports: Yes (will need to clean these out of both m&f printed threads)
• Resulting 'tightness': Firm

alnis

@Argo glad to hear it is helpful! One thing to note: for supports, you can add a "support blocker" in Cura (and probably other slicing software) to prevent supports from gumming up the holes if you want.

https://support.ultimaker.com/hc/en-us/articles/360012869379-How-to-block-support-generation-in-Ultimaker-Cura

Evan_Reese

FWIW I do it both ways, but I tend to actually add the clearance to the shaft and hole first, then use two thread-creator features for the male and female threaded parts. It keeps the thread profiles a bit more accurate, even though it costs more in modeling time.