Yet Another Post About Modeling Threads

[Anonymous]

Hello Everyone,

So I've got this part and I've attempted to model thread onto a shaft (some thread dims assumed) equivocating roughly to 1-8 UNC. I did this once with a normal coil followed by a tapered coil to simulate the "trailing threads" or however they may be more appropriately refered to however I was not completely satisfied with the result due to 1. unfavorable geometry at the start of the taper and 2. thread profile not perpendicular to path.

So I decided to try to implement something that I've done in the past and create a 3D sketch to draw a path and make a plane for the profile and sweep. Everything seems to work fine until I create the sweep cut when I get an error saying that it doesn't produce a meaningful result. Additionally, I'm able to sweep it as a new solid, then if I try to combine cut, I get an error stating that it doesn't result in a change of geometry (or something like that).

I've attached the part file. All geometry and sketches are controled by user parameters.

Anybody know why I'm getting these errors while trying to make this sweep? I kind of just did this for fun... just to see if I could get it to work and look right. So no rush.

Thanks,

[Anonymous]

SO! I may have spoken a tad too soon.

I switched the helical curves to represent the ID of the cut rather than the OD and the cut worked. I would think that since the OD is so much wider than the profile, that this would not be the source of the issue.

Any other thoughts on why the OD helical sweep path wouldn't work?

Corrected model attached. Feel free to use it for... stuff... if you want. User Param controlled threads could turn out to be useful I guess.

[karthur1]

Will,

I am working with your first model.  Guess you are looking for the threads to do this.

The reason that it was giving you an error when you tried to do it all with one sweep was because of the transisition where the two 3D paths joined.  I swept the threads as a seperate body, then used the combine cut tool.  Before I did the combine cut, I had to remove those faces were the two coils intersected.  Thats what the error was telling you.... its just worded weird.

What thread is this anyway?

Kirk

[Anonymous]

Yup, that looks about right. You'll see that in the second model I uploaded. What I would really like is for the tapered portion to be tangent to the original and taper out correctly but I may be asking too much. I tried fooling around with the coil ends in the options but they're not something I fool around with much and in the 3D sketch I was having difficulty telling exactly what my changes were doing.

I opted to revisit that particular issue at a later time. I wanted to double check my thread profile to see how accurate it was and as it turns out, it could use a little brushing up. With that said, I intend to brush. Which is what I'm working on now.

Thank you for your reply. I appreciate that you were able to troubleshoot that quickly. I will, however, continue to improve the model based on what I mentioned above because I'd like it if (again... may be asking too much) it could be done in one sweep.

[karthur1]

As far as the two curves being tangent ... It looks like either method will produce that.  You can check the smoothness by doing a zebra analysis (View>Analysis).  If it was not smooth you would see a edge here from black to white.

Just for simplification, I would use the second method where the curve followed the inside diameter of the threads.  Less things to go wrong later down the road.

Kirk

[Anonymous]

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@karthur1 wrote:

As far as the two curves being tangent ... It looks like either method will produce that...

Just for simplification, I would use the second method where the curve followed the inside diameter of the threads... 

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Yeah they both produce that result, and it makes perfect sense that they would. The path goes from that straight coil into a coil with a set taper, there ought to be a corner (ever so slight though it may be). I'm trying to think of a way to remedy that... but it's not the highest priority on my list. I'm working out the thread profile right now. Trying to come up with a cleaver way of taking care of the amount of the material that is completely removed from the nominal OD of the shaft. In the case of a 1" nominal diameter, the amount of material removed from the outside of the shaft on the threaded area is 0.125*(0.5*pitch*sqrt(3)) for UN threads assuming the angle is always 60 deg (which I don't know enough about threads yet to confirm or not).

So I'm working on trimming that material for the threaded length without getting any strange resulting geometry.

[graemev]

Check out Machinery's Handbook for thread profile data.

A simpler, and perhaps more real world, solution might be to cut the thread full depth to the total thread length (including imperfect threads in the runout area) and then extrude-add a cone for the imperfect zone.  If you look at a tap or a threading insert, you will see the corresponding geometry on the tool.  Only in single-point threading would the threadform's root "retract" to the OD of the shaft, per your current model.

[Anonymous]

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@graemev wrote:

Check out Machinery's Handbook for thread profile data.

A simpler, and perhaps more real world, solution might be to cut the thread full depth to the total thread length (including imperfect threads in the runout area) and then extrude-add a cone for the imperfect zone.  If you look at a tap or a threading insert, you will see the corresponding geometry on the tool.  Only in single-point threading would the threadform's root "retract" to the OD of the shaft, per your current model.

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Machinery's Handbook is in hand 😉 I'm just adjusting the profile.

On your second point... maybe I could do that. However, as previously mentioned, I've somewhat tasked myself with doing this in one feature (sweep) however, I'm not opposed to the suggestion. Especially if that's how real world tapped threads would look.

Interesting... I'll definitely keep this in mind moving forward. I was also considering adding the potential for a relief groove instead of "retracting" the root.

[JDMather]

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@Anonymous wrote:

... 2. thread profile not perpendicular to path.....

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Threads are a case where the profile is not perpendicular to the path.

If you go out to the shop floor and use a single point tool to chase a thread on lathe you will discover this.

Also, what thread specification are you referencing?  I thought an ACME was 29°.

[Anonymous]

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JDMather wrote:

Threads are a case where the profile is not perpendicular to the path.

... 

Also, what thread specification are you referencing?  I thought an ACME was 29°.

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Good to know! Like I mentioned in one of my other posts in this thread, I'm not super familiar with thread design. I've seen it cut on a lathe but still thought maybe there's a way for the profile to be perpendicular to the path.

I don't think I've uploaded a new part file since but I've updated my sketch to more accurately represent what the Machinery's Handbook describes as a UN EXTERNAL THREAD. I've been working toward/with a 1-8 UN thread. I'll reattach my latest part file with the updated profile. I'm currently trying to trim the extra meat that that the nominal diameter has over the thread OD while still keeping the model aesthetic and as close to 'real' as I can. Thoughts on that process?

[Anonymous · Accepted solution]

Not to keep reviving this but I got the iFeature to do all of the things I wanted it to. It took some time and patience but I got there. If anybody who reads this would be interested in having it, let me know. I'm unable to attach the .ide in the forums but here's a video and a list of what the ifeature can do:

Accurately model UN, ACME & NPT External AND Internal threads. Diameter is picked up from the part file and applied to the thread so that when the diameter of the part changes, the thread diameter changes with it. Users have the option of choosing the way the thread ends between 3 options: None (thread abruptly stops), tapered (thread profile tapers out of material) and relief groove (material cut away so that threading tool can leave threads and be retracted without removing more material). Users also have the option of choosing if the part is meant to be fully threaded, in which case theuser must ensure that the working thread length matches the part length.

[karthur1]

Will,

I would like to take a look at it.  Can you put the .ide in a zip file and post it?

Kirk

[Anonymous]

Sure thing. The only other thing I noticed after having already posted the video was that the threads were in the wrong direction. In other words, they didn't follow the righty-tighty, lefty-loosey rule.

But that has been fixed as well as the .ide updated.

[Anonymous]

Whatcha think Kirk?

Does it stand up to the test?

[karthur1]

"What-if" you actually needed a left-hand thread?  Pretty cool iFeature, though.

[Anonymous]

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@karthur1 wrote:

"What-if" you actually needed a left-hand thread?  Pretty cool iFeature, though.

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Oh I'd just cry.

To be honest, I don't know if it's possible to have a variable determine that... I haven't tried it but... yeah I don't think it's possible. I mean not without just creating a macro that draws the whole thing where you can change it with VB coding.

I don't think I can control that toggle button in the coil(s) with the change of another variable. If you know of a way, I'd be happy to allow such a thing to be an option for the end user. Otherwise I would likely make a second iFeature that does left-handed thread. It was easy enough to fix it to right handed thread when I had it backwards before.

The biggest challenge with creating this ifeature was having the equations for my key parameters (say cut profile height) change based on if you pick 1, 2 or 3 for the thread type. And change correctly. There's no iLogic nor VBA involved. I don't think I'm able to use those in an ifeature and if I am, then I made this alot more diffcult than it needed to be.

[karthur1]

Will,

I think its beautiful like it is.  It would cover 99.9% of what I would need this for.

Kirk

[Anonymous]

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@karthur1 wrote:

Will,

I think its beautiful like it is.  It would cover 99.9% of what I would need this for.

Kirk

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You're too kind. But thank you. It took a good bit of time to get it to work properly.

If I'm being perfectly honest though, there is one scenario in which it throws an error and I'm not sure why.

Using the iFeature, put internal and external threads on a part using the same end face for the plane. Like having internal and external threads on the same end of a pipe for example. An error is thrown when switching to and from NPT threads. It seems to lose track of the face for the internal threads. I don't really know why. It can be fixed pretty easily by redefining the face through editing the ifeature but I don't know why it happens in the first place.

[DavidKuhlmann]

To make a left hand thread can't a right hand thread part be derived as a mirror about the X-Y plane?  I apologize, my samples are in 2016 and I just noticed you are using 2015.

[Anonymous]

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@Anonymous wrote:

To make a left hand thread can't a right hand thread part be derived as a mirror about the X-Y plane?  I apologize, my samples are in 2016 and I just noticed you are using 2015.

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I mean making a right hand thread on a part is very simple and yes, you could use the thread ifeature I've made and derive it into a new part file and mirror-removeoriginal. I think what Kirk was saying and what I was referring to was having the option of choosing "Left Handed" or "Right Handed" threads within the ifeature, thus cutting out the step of applying the threads to a part then deriving and mirroring.

What you've suggested would work (though I cannot open your part files) for creating left handed threads though there would still be the obstacle of whether or not that mirror would effect the overall part negatively (in other words, the part needs to stay the same but just the threads need to be mirrored).

Then again, I could just have another iFeature where the thread is cut in the left-hand direction rather than the right. It's a simple switch since all the work to make that iFeature possible has already been done.