Inappropriate thread error

[Anonymous]

I am reverse engineering a part for the purposes of inclusion in a 3D printed plastic mockup of an assembly.  Unfortunately, when it comes to duplicating a portion of it that is an external thread, Inventor gives me an "inappropriate thread" error.  The thread looks like it is still in the part in the modeling window, but in the model tree appears the little "i" error icon, and when I save the file as an STL the thread isn't rendered at all.

Does anyone have advice on what to do about this?  I am pretty sure the thread is the same as in the existing part.  I don't know what Inventor's problem with the thread is, and I wish it would just make it anyway.

[dag_h]

In my experience I get the error when I use a thread size that is far from the modelled diameter size. I can't say I have a fix though, beyond modelling the diameter to more closely match the thread size, perhaps.

[Anonymous]

The size you need must not be within the available library of standard sizes that inventor has to pick from.

What size thread is it? Would having modeled threads solve the problem?

Which Inventor are you using?

[JDMather]

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@Anonymous wrote:

...and when I save the file as an STL the thread isn't rendered at all.

Does anyone have advice on what to do about this? ....

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If you want threads in STL model - you will need to model them, not use cosmetic threads.

Attach your file here.

[Anonymous]

Ah, I wasn't aware of the distinction between modeled and cosmetic threads.  The Inventor I am using is 2015.  Here is the file!

[JDMather]

Workplane 1 is a duplication of the YZ plane and therefore not needed.

You Ø6.18mm cylinder is way too small for a 5/16 thread.

If you want real threads - you have to model them - see this thread (pun intended).

[Anonymous · Accepted solution]

Dang, JD got back here before I could. Yeah, if you want to see thread elsewhere or for renderings or whatever, you'll need to model them. The thread JD points to is a good reference on how to model them.

I'm left with the impression, however, that if you've just applied the thread tool at that location, you're not entirely certain of the size thread on the part. Assuming the 5/16-18 UNC that Inventor attempts to apply is correct, you would need to add the material at that location then cut away the threads.

Instead of just adapting what you already have, I'm going to redraw it from the ground up for reference. Everything here can be created by 1 sketch and 3 features and be more flexible than it currently is. See attached for reference. You're model is still there and I added real thread to it before deciding to rebuild. But that way you can see the two side by side.

[JDMather]

A work of art, a thing of beauty.

Your single sketch profile reveals a very thin section that might have been missed unless the OP does a Section View.

[Anonymous]

I'm glad you like it JD. That thin portion had me raising an eyebrow too but that's above my paygrade 😉

[Anonymous]

This has been really useful and I have learned a lot from this thread.  Unfortunately, I don't know anything about iFeatures, so I'm not sure how to add the extra clearance I need for 3D printing (like in the linked thread).  Any quick advice on how to do this with the iFeature might be useful, but anyway, thanks for the great responses.

[dag_h]

The extra material removal as JDMather modelled the threads weren't iFeatures, as far as I can recall, they were just a sketched feature.

[JDMather]

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@Anonymous wrote:

...I don't know anything about iFeatures, so I'm not sure how to add the extra clearance I need for 3D printing .....

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No iFeatures used in the example I demonstrated.  iFeatures is simply a way to automate future work.

I suggest you give it a try yourself and post back if you run into trouble.  In addition to the thread feature - I recommend taking a second look at these two angles.  When I worked out on the shop floor I had to make special tools when I got a design like this. Upon interrogation of the designer - I would discover that the angles weren't critical.  Especially the 90° I would examine to see if a standard drill bit 118° would work as that would make it a much less expensive feature to manufacture.

[Anonymous]

Well, I have made a thread pretty much the way you showed in your video.  However, my thread cutout seems to be too deep or my numbers are wrong in general.  I looked up what a #18 thread is in terms of pitch.  It gives me 1.411 mm.  Anyone know what I've got wrong?  Sorry, this is my first time really working with threads.  I'll attach the file.

[Anonymous]

valbotany,

Sorry about the inclusion of the ifeature. So long as it is in that part, you should be able to adapt it however you like by editing it in the browser but I would, like the others also recommend drawing it by hand just for the practice.

The file you attached has a sketch but no sketched geometry. But it should be pretty easy to figure up. 18-UN threads have 18 threads per inch. If you're converting that to mm, then (1/18)*25.4 = 1.411. So good. Seems your source was correct though when you're doing something like this, I feel as though I ought to suggest simply entering the value in it's native unit instead of converting elsewhere and then entering the number. For example, my company uses feet and inches for everything, however, every once in a while we get client supplied drawings in metric units. Instead of converting them, I can open a part with units in inches and simply type in "25.4mm" where I need to and inventor will apply the unit I specify to the value.

At any rate, if you're looking to 3D print this and thus need to modify the threads, there's probably 1 of 2 ways you can do this: The exact method JD showed in his video should work. I can think of no reason it wouldn't or, if you have the material available, the iFeature could be used so long as either the male threads are slightly smaller than nominal or the female threads are slightly bigger... or both. I'd still suggest drawing the threads though.

Could you repost the file with the attempt you had at drawing the threads yourself?

[Anonymous]

Sorry, I don't know what happened with the last file I uploaded, but here is a correct one.

[JDMather]

Are you measuring an actual part?

If so, can you take picture of the part looking directly at it and attach the picture here?

This 5.xx diameter will need to be reduced.

I also recommend that you add Chamfers before the Coil feature.

The method I demonstrated uses a full depth on the triangle, where if you look at the reference you posted earlier - they don't use full depth.  That might help the depth of your cut.

I forgot to mention - the extra workplane and axis are not needed - use the Origin workplanes and axis when possible.

[Anonymous]

To further clarify the full depth triangle dilemma:

Look online and you'll find UN thread profiles that look like the above image. Note the equations used. You could use this profile and the method JD suggests for making sure the 3D printed version doesn't bind up and you should be on your way. (Also chamfer the ends ;))

[Anonymous]

Sorry to ask a question which is a little more in the direction of pure engineering rather than Inventor, but can anyone explain why there is the offset/dimension "d84" in the preceding image?

Sorry to be such a beginner, but I would think that the external diametric dimension of the male and female parts would need to be the same.  Intuitively, it seems incorrect to me that the cut on the male part should be offset outward, the way it seems to me to be with that dimension in there.

Any insight on this kind of thread stuff would be greatly appreciated.  It would be great to really know what I am doing in the future.

[JDMather]

What country (standards) are you in?

I guess it doesn't matter as metric threads should be standard world-wide,

but I am referencing the Machinery's Handbook.

This could end up being quite a long discussion, I am reluctant to continue, but it is important and I can use the results of the discussion in my classroom.  Do you own a Machinery's Handbook?  I guess these days I could probably find the same diagrams on the internet.  This is already starting to sound like work... and I have other work I really need to get done....

...cut threads  ...rolled threads... limits and fits.... 

Do I need to find an internet reference - or do you own a Machinery's Handbook?

Once I know we are working from the same reference - we can walk through all of this step-by-step.

[Anonymous]

I do own a Machinery's Handbook 29th Edition.  I am in Europe, so I use metric the most, but this particular part and many others I need to work with are imperial, so I really need to use both.

Thank you very much.  Particularly with how much I use 3D printing, it'll be invaluable to know this stuff.