Threading for 3D printing

[voltagearc]

I'm very new to Inventor (have worked with other modelling softwares) so I still don't quite understand how to create a physical thread versus a "visual" or cosmetic thread. I'm currently modelling a supressor prop (which I will 3D print in plastic) for an airsoft gun and am making two parts 1) the supressor, with a threaded hole to stick the barrel into and 2) an adapter, essentially a cylinder with a hollow smooth inside and a threaded outside which will fit over the unthreaded barrel of the airsoft pistol and allow for me to use the threads. My confusion is that, after exporting my objects as STL files, the threads do not appear, despite my using the hole-> thread command and thread commands. Could anyone explain how to get physical threads for 3D printing. Threads are ANSI Unified Screw Threads 11/16-12 UN 2B and 2A respectively.

[SBix26 · Accepted solution]

There is an add-on for Inventor from CoolOrange, I believe, which will cut actual threads.  Or you can do it yourself by sweeping the proper thread profile along a helical path.  Inventor's threaded hole feature does not cut actual threads, since helical surfaces are data-intensive and having a large number of them in a model would bring Inventor to its knees.  Therefore, the thread data is saved with the hole feature, and a cosmetic appearance is added to the threaded face so it's easy to identify visually which holes are threaded.  Obviously this isn't too helpful for 3D printing, so you have to cut your own-- but be sure to add extra clearance to the thread, since printers aren't nearly as accurate as machined threads.

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Sam B
Inventor Pro 2019.0.1 | Windows 7 SP1
LinkedIn

[johnsonshiue]

Hi! Here is the link to the free app from coolOrange.

https://apps.autodesk.com/INVNTOR/en/Detail/Index?id=2540506896683021779&appLang=en&os=Win64

Many thanks!

[Anonymous]

I've been using Cool Orange for several years to print threads in our Stratasys Objet 500 C3 3D printer.  They've always been perfect.

I just upgraded to Inventor 2020 and now the threaded holes are too tight.  If I chase them with a tap they chip out.  I thought I could just make the holes .010" bigger but then I can't assign the thread I want.

my process.  Make the hole the Major Dia of the thread I want.  ex #10 = .19" .  Then assign the thread to that hole.   Using Cool Orange add physical thread.  Too Tight!

Any suggestions?

[-niels-]

Have you ruled out any other possible causes?
If you make the same model in your previous version of inventor, is the thread correct?
Are your slicer settings still the same?
Is your printer still calibrated properly?

You could try to compare the cool orange generated thread to a manually drawn thread in the same model.

[Anonymous]

Parts modeled and saved as a .stl prior to the Inventor 2020 upgrade are still ok. 

[TheCADWhisperer]

If you model your own threads - you can take absolute control.  🤔

[waconiabarrett]

I'm having the same issue.  Cool Orange was the "coolest" plugin, but now every thread I print (male and matching female) prints too tight.  Nothing else has changed with printer or slicing software.

Other than modeling them manually, any ideas or solutions?

[EverhardDawnwood]

I know its an old thread, but theres another option and thats Fusion360 which can natively do modeled threading.
F360 can import ipt files directly and you can easily do your threading in that.

Its a workaround as some info is lost when saving the file as ipt in F360 and opened with inventor, but what I did was do the whole part in inventor, then as the final step, opened it with F360 and did the thread I wanted.

It means that if I ever change the part, ill have to redo the thread with F360, but it takes just seconds to do.

What I dont understand is, how come even inventor 2022 (I just upgraded from 2019 today) doesnt have that same thread modeler that F360 has, I mean both are Autodesk products and F360 is being like a "light" version of inventor as I see it?

[edmccracken]

In my testing, I found:

1. The hole for the nut threads must be sized to the nominal thread size (0.500" for 1/2", etc.)
2. The shaft for the screw must be a smaller size, such as the minimum outside diameter of the screw threads. (0.485 for a 1/2" screw). This makes the screw a bit smaller than nominal, and is the way real screws are made. I size this ~95-98% of the nominal screw size.
3. Once CoolOrange is applied to the nut, you need to go back in and cut away the peaks of the threads with a simple circle extruded cut down the center. The CoolOrange thread peaks are a bit too tall and make for a super tight fit. I shave out about 0.025" diameter larger than the max inner diameter. 
4. Add a small 45° chamfer to the edges of the screw and nut threads. You need to Combine the solids after CoolOrange is applied, or cutting into the threads fails.

If this method is still too tight, you can use the Direct Edit tool to offset the nut surfaces outward a bit (0.005-.010") to give more clearance. This can be finicky however, so you might want to look into modeling your own threads.

[seanlava]

Thank you for your testing data, I always appreciate it when someone answers the question that was actually asked by the OP.

[arman.sesar]

this is unfortunate, I wish Autodesk offered a native 3D thread modeler in Inventor as it does in F360. It is not always required but great for prototyping. I know solidworks offers this natively.

[-niels-]

Add votes:
https://forums.autodesk.com/t5/inventor-ideas/real-thread-modeled/idi-p/6504747

[TheCADWhisperer]

@arman.sesar 

Fortunately, modeling threads is easy.

[dtaylorZ9JTS]

JD, I know this is an old thread and I hope you'll get to see this post.  I started using Inventor in 2012.  I'm just a middle-aged guy who likes to tinker on building things so I'm not a serious student of Inventor and not aspiring to a job with it.  That kind of makes me a hack.  Back in 2012, I posted my first question about Inventor and you answered it.  Likely, back then, I was under a different user name, and it may or may not have been on this forum.  Regardless, over the years, you have helped me tremendously both directly in response to posts I've made and indirectly, like today, as I read your answers to others' questions.

I'll look you up on YT and subscribe and make some comment(s) there.  But I wanted to say this:  Thank you so very much for all the help you have given the community with your immense knowledge and experience.  You answer countless posts and that takes lots of time.  The time you took to make this video response was appreciable.  It is not possible to say enough kind words or do anything in return to honor the immense effort you have put into helping those of us who are trying to learn.  Saying "thank you" is wholly inadequate, but it's what I have.

Thank you.

--HC

[cadman777]

Just for the sake of argument, I'm adding my 2 cents' worth.

Having done 3d printing, I can say that unless you have a very expensive 3d printer, your formed threads will not print well enough to be useful. Instead, I make sure the print has an undersized hole (smaller than the root) and there's enough solid material around the hole to use a steel tap to cut the threads after the print is finished.

I've made a number of prints like that and they work great. Most of the threads were #6, #8 & #10. Some of them were 1/4-20. The print plastic was ABS. I've not needed to do this with external threads, but it seems to me that it would be no big deal when done the same way. Adequate solid plastic material will result in good thread cuts using a steel die.

So, I wouldn't waste my time making threads in Inventor for a 3d print. I'd recommend to do it manually after the fact.

[hardiebothaNLKXT]

I don't know how long ago you ventured into 3d printing, but that is a very inaccurate or dated statement and is getting more inaccurate daily. Printing a 6x1 Metric thread, which will fasten just fine is pretty easy. Sure, you're not going to torque it to 30 Nm. Many polymers don't cut well, so threading afterward is often not viable.

Another point that often comes up is "Modelling threads is easy" - sure, but it is time-consuming, and doing it in a bunch of places multiplies the time wasted on what should be trivial. JD has an excellent video on it, but it only caters to internal threads.

It should be clearly stated that this significantly complicates the model and be recommended to be done as the last step.

[gallen-ext]

Good Afternoon, Just wondering, now that CoolOrange has stopped in 2024, is there now an Inventor 2024 solution to generate threads? Also how does FEA work with threads if there is no physical form?