Adding internal threads for 3D printing that work with standard machine screw fasteners

[sinclair314]

Problem:  using the built-in internal tapped hole command in Fusion360 produces correctly modelled tapped holes for precision CNC milling tools but will usually be undersized for use with a FDM 3D printer where standard machine screws will not fit. If you want to use these holes for inserting machine screws, try the following to increase the tapped hole size so the mating machine screw will fit. Strength will depend on the fit, how long the threaded hole is and the direction of the hole relative to the direction of the printed layers.

• Place an arbitrary sized hole (probably ~ the screw size) at the place you want the tapped hole. I mainly use the Circle and Extrude command.
• Select the inside surface of the hole
• Choose Solid->Create->Threads
• Select Modelled
• Select the correct screw size (IE  0.25 in, 1/4-20...3B. This will correctly size the hole (but for CNC milling use). I use the ANSI Unified Screw Threads table which is the default.
• Choose how far into the solid the tapped hole should go. 
• You can also use the Solid->Hole command for more options
• For each internally tapped hole, select all 4  surfaces of the thread. I use Select->Window or Select->Freeform or Shift+Select to just select all 4 surfaces.
• Choose Solid->Modify->Offset Face to offset the thread faces (make larger)
• You should see "4 Sufaces selected"

To adjust the threaded hole size, enter the amount to enlarge the hole. I found -.007" (.18mm) a good starting point with most screws I use. Important - Note the negative sign which is required to make the hole larger. You should be able to hand-thread the screw into the hole without much effort or slop. Adjust the offset accordingly. Use a tight fitting thread to mimmick a locking fastener.

This works well for me in most cases for screw-fastening 3D printed objects as it's much less effort than adding screw inserts ... but use appropriately. This technique can also significantly strengthen a printed object by creating one or more long tapped holes and adding an appropriately sized screw (or threaded rod).  By cutting a screwdriver slot in the end of the rod, you can bury it out of sight. This can add much strength to the printed object in the weaker direction, normal to the printed layers.

Happy tapping!

[laughingcreek · Accepted solution]

offsetting all 4 faces will cause the peak face to get smaller, and the valley face to get bigger, resulting in a weaker thread (blue is the tapped hole)-

if you offset the peak face , the valley face, and just ONE of the side faces, you will maintain the designed size of the peak and valley faces, resulting in better thread performance-

[MRWakefield]

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@laughingcreek wrote:

offsetting all 4 faces will cause the peak face to get smaller, and the valley face to get bigger, resulting in a weaker thread (blue is the tapped hole)-

if you offset the peak face , the valley face, and just ONE of the side faces, you will maintain the designed size of the peak and valley faces, resulting in better thread performance-

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I'm very pleased to see someone else correcting misleading guidance on this as I have become quite frustrated correcting others on this. I even put together a document ready for next time anyone recommended offsetting all four faces!

[TheCADWhisperer]

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@sinclair314 wrote:

• I mainly use the Circle and Extrude command.

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Why do these extra steps?

What about lead-in chamfer for the thread (as done in the real world)?

[sinclair314]

Good suggestion. But I'm guessing if Fusion thought it was a useful addition it would have been included in the Hole or Thread command (but that's a silly assumption, I know). I am a lazy engineer who was looking for a quick way to add usable (read usable and not perfect) threads and avoid adding screw inserts in most cases. ... and that's the story I'm sticking to 🙂

[sinclair314]

Thanks all who responded, good suggestion. I think that, considering the popularity of FDM printing and the number folks who have been looking for a usable thread solution, Autodesk should consider putting in an input for this in its thread-related commands. Also, how to quickly select the right 3 faces? (Group-selection is fast). Thx again.

[TheCADWhisperer]

@sinclair314 

Ask questions about the lead in chamfer.

Almost everyone gets it wrong.

[MRWakefield]

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@sinclair314 wrote:
Thanks all who responded, good suggestion. I think that, considering the popularity of FDM printing and the number folks who have been looking for a usable thread solution, Autodesk should consider putting in an input for this in its thread-related commands. Also, how to quickly select the right 3 faces? (Group-selection is fast). Thx again.

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Having the ability to add an 'offset amount' would be useful to many that 3D print their threads and there would be no confusion then over which faces to select. The offset could just be added or subtracted to/from to the Major, Minor and Pitch diameters in the model automatically. I'm not sure there's enough incentive for AD to add this particular feature though so I wouldn't hold your breath!

There is an alternative method which might work if you want a constant amount added or subtracted to a complete thread series and that's by using my Fusion 360 custom thread utility (linked in my signature). This will allow you to take an existing thread file and add or subtract a constant amount to/from all of the sizes. It is Windows only though so if you're on MacOS I'm afraid you're out of luck.

[sinclair314]

I have experimented with the above suggestions and, for the most part, Face Offset for 3 of the 4 faces appear to mostly work - thanks.

One problem I see is for a threaded hole completely through a rectangular block at right angles to one of the faces. An offset too large (that I need) will make threaded hole completely disappear.  (IE an Ansi #6-32 threaded hole enlarged with a Face Offset of -0.015").  How to rectify this anomoly?

A question if I may:

- How do you suggest I select these 3 faces? This is how I do it now:

    - Group-select all 4 faces of the threaded hole

    - Zoom in on one of the threaded holes and carefully de-select one of the inclined faces.

    - Apply the Face Offset

[etfrench]

How would you print a 6-32 thread with faces offset 0.015" using an FDM printer?  Can you even print an accurate 6-32 thread when the threads are only 0.36mm thick? 

I think the thread dialog should not allow an obviously invalid setting.

What do you think Fusion 360 should do when the faces are offset more than the thickness of the thread?

[sinclair314]

Great question.  Accurate ... no, compared to a proper milling tool.

This works for me and saves me a lot of time. 

Obviously the thread pitch, thickness of the layers, printing direction of the threaded hole wrt hole, size of nozzle, layer adhesion, type of material, elephant foot effect, time of day, etc. will affect the quality of threads and holding power. I do this fairly effectively (IMHO,) by using either the sketch circle+extrusion+Create Thread or the Solid-Create Hole command then select "Ansi Unified Screw Threads" and select #6-32. Choose the desired tapped hole geometry, depth of hole, shoulder, chamfer, etc and be sure to select the "Modelled Threads" checkbox.  After that, you must select the correct 3 (out of 4) thread surfaces and use the Solid-Modify-Face Offset command to specify how much to offset. You can select all 4 faces by a Window or Lasso tool, selecting the threaded hole. Then zoom into the hole and using CTRL+mouse button, deselect one of the angled faces, leaving 3 faces selected. Then select Solid-Create-Face Offset and apply an offset, "-0.015" in this case. Be sure to use a negative offset # to make the hole larger.

It sure would be great, given the popularity Fusion360 has with the 3D printing crowd, to add this offset to their thread command window.

I was corrected in my earlier post by folks much more experienced than me to make sure to select the correct 3 (out of 4) surfaces (see replies).  Remember that an FDM printer's output is not a very accurate CNC machine compared to normal threading equipment.

When in doubt, use a plastic thread tapping tool in a correctly sized (simple) hole. Make sure to add enough wall loops to accommodate the cut threads. Or you can always use a heated thread insert for good strength in the "pull" direction.

Most situations of modelled threads hold fine for my use and are simple and easy to produce with no additional labor after the print.  

By offsetting the thread dimension, I believe I'm asking Fusion to scale the thread dimensions orthogonal to the hole axis and not the thread pitch. Can anyone add credence to this?

Fusion360 doesn't allow an invalid setting if you know what standard-accepted ANSI specs to enter. What is produced by a garden variety FDM printer can't reproduce an ANSI standard thread per what you suggested. The strange behavior I was referring to was me trying to change the printed thread size beyond the ANSI standard range. 

Good luck    mike

[MRWakefield · Accepted solution]

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@sinclair314 wrote:

I have experimented with the above suggestions and, for the most part, Face Offset for 3 of the 4 faces appear to mostly work - thanks.

One problem I see is for a threaded hole completely through a rectangular block at right angles to one of the faces. An offset too large (that I need) will make threaded hole completely disappear.  (IE an Ansi #6-32 threaded hole enlarged with a Face Offset of -0.015").  How to rectify this anomoly?

A question if I may:

- How do you suggest I select these 3 faces? This is how I do it now:

    - Group-select all 4 faces of the threaded hole

    - Zoom in on one of the threaded holes and carefully de-select one of the inclined faces.

    - Apply the Face Offset

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I don't know for certain why offsetting by more than about 0.015" causes the hole to disappear as I can't see why it shouldn't work. My guess is that in the background Fusion offsets the faces one at a time and the intermediate geometry becomes messed up (that's a technical term 😉). To get around your problem you can split the offset into two stages: Offset once by 0.01" then add a second offset of 0.005" (bizarrely once you've applied the first offset you can even apply a second offset of 0.05" without a problem!). I've tested this and it works. Alternatively I have created an internal ANSI Unified thread file with +0.03" on the Major, Minor and Pitch diameters (see attached).

To answer your other question: I select the three faces by clicking the first one than ctrl-clicking the other two, but your method of selecting should work the same.

Hope this helps.

[sinclair314]

Thanks!
Yes, I found the .xml file for the Fusion ANSI thread data and added a separate "FDM..." item to all my common screw sizes by modifying the respective diameters. These special thread names come up when I open the standard ANSI thread sizes in Fusion's thread tool. But for some (operator error?) reason, these didn't work well.

I am basically a lazy DIY, do-it-quick-easy and good enough user when printing in the non-deterministic plastic FDM world. The Face Offset way for threads seems to work for me now with minimum effort. (as long as I select the correct surfaces and remember to enter a negative offset (!). It also appears that a constant offset of around -0.013" appears to work for most of my thread sizes (and PLA). I have an electronic force gauge I will eventually employ to test the thread integrity at fracture for various offsets and materials. But that's for a later time.

I occasionally use this technique to add stiffness to parts by including threaded holes and installing long metal screws or threaded rod. This is especially useful if stiffness is needed in the normally weaker axis, perpendicular to the FDM layer plane.

[MRWakefield]

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@sinclair314 wrote:
Thanks!
Yes, I found the .xml file for the Fusion ANSI thread data and added a separate "FDM..." item to all my common screw sizes by modifying the respective diameters. These special thread names come up when I open the standard ANSI thread sizes in Fusion's thread tool. But for some (operator error?) reason, these didn't work well.

If you've edited the original Fusion 360 file rather than edited a copy I'm pretty sure it gets overwritten with the next Fusion update, so you'd lose your edits anyway. If you do use any custom thread files you would need to move them with each update so I always recommend the ThreadKeeper add-in. This takes care of copying your custom thread files whenever Fusion gets an update. I also recently added similar functionality to my custom thread app mentioned in a previous post but ThreadKeeper is an install-and-forget solution rather than mine which is a bit more user-assisted.

I am basically a lazy DIY, do-it-quick-easy and good enough user when printing in the non-deterministic plastic FDM world. The Face Offset way for threads seems to work for me now with minimum effort. (as long as I select the correct surfaces and remember to enter a negative offset (!). It also appears that a constant offset of around -0.013" appears to work for most of my thread sizes (and PLA).

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That's fine, at least we've determined that two smaller offsets work if one larger one doesn't!

[adminA9Z6M]

Engineers are generally busy, not lazy. Our time is a valuable commodity that cannot be consumed with difficult, slow , or inefficient CAD work flows. Any improvement in workflow for threaded features, or any features for that matter is important. Just wanted to mention that 🙂

[adminA9Z6M]

I model threads all the time in other CAD packages. They all have the ability to do helical sweeps of some sort. Fusion has a hacky work around using coils but its not great. If Fusion improved helical operations you could just cut or extrude sweep your own custom sized threads with no issues. This is something that is quite necessary in 3DP as well as other custom threadform machining rather than trying to use the thread tool.

[sinclair314]

Thanks for the thoughful input. I will take issue somewhat with the lazy aspect. Many times that behavior develops into a valuable time-saving tool when done correctly. Maybe I should redefine "lazy" to searching for a more time-saving method?

I am a relative newbie at this CAD and 3D printing and am learning all the time so any time-saving method (if it works) is valuable to me.