Christopher Estelow wrote:

 

Has anyone ever seen this one before? I opens the file but I'm unable to do anything because all the commands are grayed out.

 

Chris

It was made with a version newer than what you opened it with.

Christopher Estelow wrote:

 

Has anyone ever seen this one before? I opens the file but I'm unable to do anything because all the commands are grayed out.

 

Chris

As Danny Edwards mentioned, if you're on the last SP of 2018, you're permitted to open SW2019.

Cool.....every other time I tried to open a future version it just had the pop-up.

Chris

Thanks for the help with the spotface, it really does help
Any idea about my question regarding executing the production quality threads?
Ive attached it as a parasolid as someone suggested to the original post

Hello.

I am trying to implement a 1/16" NPT thread on a curved surface.

I have used the hole wizard and a tapered tap option to tap a hole where I want in tapered pipe tap, but since it's on a curved surface SW won't allow me to thread a curved a surface.

This leads me to believe that I may need to tap and thread the hole manually, but I am unsure of how to go about doing that to a production level standard (as I understand the thread profiles are not to be used for production quality stuff, which is what I am trying to do)

Does anyone have any idea where I could start going about solving this issue?

I am very new to the aspect of creating production-quality threads, let alone non-linear NPT tapered thread so I am trying to do it correctly from the start.

I have attached a model of the surface I am trying to thread.

Thanks in advance for any help/direction.

Hello,

If I understand correctly, you want actual 1/16 NPT threads cut into your part.

The Thread command doesn't do NPT I don't believe.

So I think you'll have to find a 1/16 NPT pipe nipple (any NPT fitting with a male thread) as a 3D model.

Locate this model into your part per an engagement standard, such as:

Basic Dimensions, American National Standard Taper Pipe Threads, NPT, (ANSI B2.1-1968) 

Then do a Combine>Subtract.

I went to McMaster as they have NPT 3D models, but their smallest size is 1/8 NPT.

Kevin

Why do you want "production quality threads"?  If you spot-face this cylinder, you aren't going to have enough wall thickness left to produce a sealable "production quality thread".

I do this all the time, work in plumbing and create 3D printed prototypes that require production quality threading. From my experience, McMaster Carr 3D models are actually inaccurate - when printing a McMaster file, often something will be just barely off to prevent you from using it in a prototype.

You have to use the helix and cut sweep command instead of the thread tool to create a production quality thread. NPT threads taper at angle of 1.7899 degrees, and each size has standard diameters. You can use McMaster parts for reference, but ultimately just take a look at the wikipedia page here: National pipe thread - Wikipedia

Sketch a circle with diameter equal to the effective thread diameter if it's an internal thread, or actual outside diameter if external. Create a tapered hole (1.7899 taper angle) from this sketch. Create a tapered helix with the desired height and pitch from this sketch. In your case, the pitch would be 1/27 threads per inch. Ensure that the orientation is correct (clockwise vs counterclockwise, typically threads are clockwise but you may have to switch the orientation depending on the way the model is built) Sketch the thread profile on a plane coincident with the axis of the helix and the beginning of the helix, and pierce the sketch to the beginning of the helix. (You can google how to derive dimensions for thread profiles, too much to explain here) Ensure that you add a taper to the thread profile, see McMaster threads for reference. Then cut-sweep it along the helix. Also, add a chamfer to the edge of the appropriate length. I usually do my helix, sketch the thread profile, add the chamfer, then sweep the cut.

Thanks for the help, I am trying to prototype some threads, and 1/16 NPT is one of them among other things like AN fittings.

I appreciate this help very much, ill give it a crack

I am very new to this so the whole McMaster thing is something I've never heard of, thanks for mentioning it.

I would print the part with just a thru hole and then cut the threads into it.  That way you are guaranteed it will be the right size.

Chris

If the proportions are correct on the image you posted, your wall thickness is only 1/8".  For a 1/16-27 NPT thread, you are already short of 4 threads engagement.  Spot face it and you're in the neighborhood of 2 threads.

Josh Brady wrote:

 

If the proportions are correct on the image you posted, your wall thickness is only 1/8". For a 1/16-27 NPT thread, you are already short of 4 threads engagement. Spot face it and you're in the neighborhood of 2 threads.

For me I would punch the hole and add a pipe Nipple of the thread size he needs to their would be enough threads.  But not sure I've even seen one that small.

I would definitely recommend what David said if the walls are too thin.

Chris

Kevin Chandler wrote:

 

Hello,

 

If I understand correctly, you want actual 1/16 NPT threads cut into your part.

The Thread command doesn't do NPT I don't believe.

 

So I think you'll have to find a 1/16 NPT pipe nipple (any NPT fitting with a male thread) as a 3D model.

Locate this model into your part per an engagement standard, such as:

Basic Dimensions, American National Standard Taper Pipe Threads, NPT, (ANSI B2.1-1968)

Then do a Combine>Subtract.

 

I went to McMaster as they have NPT 3D models, but their smallest size is 1/8 NPT.

 

Kevin

It doesn't specifically say NPT here, but if you drop it onto a part:

Dan Pihlaja wrote:

 

Kevin Chandler wrote:

 

Hello,

 

If I understand correctly, you want actual 1/16 NPT threads cut into your part.

The Thread command doesn't do NPT I don't believe.

 

So I think you'll have to find a 1/16 NPT pipe nipple (any NPT fitting with a male thread) as a 3D model.

Locate this model into your part per an engagement standard, such as:

Basic Dimensions, American National Standard Taper Pipe Threads, NPT, (ANSI B2.1-1968)

Then do a Combine>Subtract.

 

I went to McMaster as they have NPT 3D models, but their smallest size is 1/8 NPT.

 

Kevin

It doesn't specifically say NPT here, but if you drop it onto a part:

I thought the OP was looking to get a cut thread modelled in? Yes?

HW taps are cylindrical/conic only, true?

Kevin

Kevin Chandler wrote:

 

Dan Pihlaja wrote:

 

Kevin Chandler wrote:

 

Hello,

 

If I understand correctly, you want actual 1/16 NPT threads cut into your part.

The Thread command doesn't do NPT I don't believe.

 

So I think you'll have to find a 1/16 NPT pipe nipple (any NPT fitting with a male thread) as a 3D model.

Locate this model into your part per an engagement standard, such as:

Basic Dimensions, American National Standard Taper Pipe Threads, NPT, (ANSI B2.1-1968)

Then do a Combine>Subtract.

 

I went to McMaster as they have NPT 3D models, but their smallest size is 1/8 NPT.

 

Kevin

It doesn't specifically say NPT here, but if you drop it onto a part:

I thought the OP was looking to get a cut thread modelled in? Yes?

HW taps are cylindrical/conic only, true?

 

Kevin

You are correct.   I missed that entire portion of it.  *sigh*.

Anyway, I wouldn't use the built in thread for this at all then.

Instead, if you really need the threads modeled in (99% of the time you do NOT need them modeled in), then use a sweep instead.  Start the sweep a few millimeters above the curved surface and cut inward.

Victor Carosi    ...agree, have pre sketch and simple model to reference!  (image showing sketch for spot face and surface model reference(s).. depending on the type of thread used)