Thread behavior

[Anonymous]

Hi!

I need to create the thread with the following parametrs.

But when I measure the outer diameter of the thread, the diameter is 10.752

What do I miss?

Thank you in advance

The file is attached

[mcgyvr]

Diameter of that hole is 20.752 not 10.752

I'll assume that you meant to write 20.752 and not 10.752 

And 20.752 is the correct "minor diameter" for that size according to the thread.xls file where that data is pulled from

[mdavis22569]

You're seeing the inside of the threads ...not where the outside would be ..which would be 24

[Anonymous]

Thank for reply.

I am following a tutorial.

Thr author uses revolve feature and then thread.

@JDMather told that this is not good practice and I should use the hole with a thread.

I use it, I set the above mentioned options for the thread.

but my result is different.

How do I achieve the same result.

I need the outer diameter of 24 and not 20.752

[Anonymous]

In a minute I will post a root of my question

[Anonymous]

Here it is:

This is an original

and this is my creature 

Do you see the difference between the marked areas

The angle and the length of line.

That is why I post my question.

Thank you!

[mdavis22569]

Look at my 2d ..

That's your 3d in drawing .. I didn't change it.   

Make a 2d ..like mine and Dim the hole ... 

[mcgyvr]

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@Anonymous wrote:

Thank for reply.

I need the outer diameter of 24 and not 20.752

---

tools...document settings.. modeling tab and set "tapped hole diameter" to "major" then hit apply then hit the update or rebuild all button.

Now it will be 24mm..

[mdavis22569]

me .. 1st option I'd through hole it ..and chamfer it .. (again I hate these exercises) A lot of bad practices in it

me .. 2nd option ...sketch with chamfer in it and revolve extrusion cut it out ...

[mcgyvr]

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@Anonymous wrote:

Here it is:

This is an original

and this is my creature 

Do you see the difference between the marked areas

The angle and the length of line.

That is why I post my question.

Thank you!

---

How do you think that to be made in the real world? 

Undercutting tool?

Whatever tutorial you are following is just wrong for the most part..

[swalton]

Turn on the Drill Point in the hole dialog, not the Flat Bottom option....

I agree, the tutorial is bad. 

I would model the hole with the tap-drill diameter, because that reflects how the part will be manufactured.  I don't know if a bottoming tap would be used on the real part, but the thread depth should be modeled correctly.

Is this a tapered pipe thread, or is there some other method of sealing the fluid in the valve?

[Anonymous]

These tutorials are bad for making you create things using bad behavour.

This is your part

In order to make this part you should do it in the same manner as if it where made.  I am assuming it is made from round bar turned on a lathe.

First choose your available material.  Based on your 39mm OD shown 2" round bar shoud do it.  Your first Sketch and extrusion should be your material, and your sketch center on the 0,0 origin:

assuming a length of 80mm

Your next operation is to turn that material down.  Select the plane that slices the material in half (because your original sketch is on 0,0

Create your skecth now to turn the material

Now Resolve using the Cut command

Add in your chamfers

Now drill in your pilot hole of 20mm

Next is to tap each end.  Choose the M24x(specified thread pitch) you will notice the drill bit has a 118deg point to it.  this is the chamfer shown on your original drawing.

As you can see my ID of the treads is not the 24mm as shown on your original but is in fact the true M24x? threads required.  Because my ID of the M24 is only 20.752 my chamfer is not as large.  To have a 24mm ID you would need to use an M26x1.5 thread pitch but even then you have 24.376mm ID

This is why the tutorials are horrible.  They teach you the wrong way to model.  In my opinon, this is the correct way and this is how they should be teaching you.  Let me know if you need help on anything else.  If you are being graded on this tutorial, do it the way I showed.  You are still using the revolve feature and are modeling the way it will be built. Any grade less than an A showed be faught as what they are teaching you is wrong

[JDMather]

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@Anonymous wrote:

But when I measure the outer diameter of the thread, the diameter is 20.752

What do I miss?

---

Pick up a real world part with a threaded hole in it and with a fastener in the hole.

Any part, but the bigger the hole the better to visualize.

Remove the fastener.

Now try to push the fastener into the hole. (without turning)

Q. Why will the fastener not go into the hole?

A. Because the hole is smaller than the fastener. Right?

So if you had in your hand an M20 threaded fastener and you tried to push it into an Ø24mm hole it would go in, but there would be no threads to hold it in the hole because the hole is too big.  The drilled hole must be smaller than the major diameter of the thread so that the threads can be cut and engaged between the two mating parts.

[Anonymous]

Thank you for all your replies!

I need some time to digest all of it.

I use this tutorial

https://www.youtube.com/watch?v=gFWAy_wnoZc

I am confused 😞
How should I learn inventor if these tutorials are bad?

I am confused

Anyway, thank you for care!

[JDMather]

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@Anonymous wrote:

So if you had in your hand an M20 threaded fastener and you tried to push it into an Ø24mm hole it would go in,  

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Of course I meant to write M24. The point is, the drilled hole must be smaller than the fastener or there would be no threads to engage.

[Anonymous]

I am 100% self taught for Inventor.  Yes, the tutorials are bad no as good as they could be.  If I were you I would use them only to see how a command works.  You need to understand how the part you are making will phsyically be made, cast/extruded/injected (grow the parts) or machine down (start with a solid and remove material). 

Get into the mind set of the fabricator/machinist and with the know how of the commands (from the tutorials) you will be make parts more efficiently.  Try and make the parts with the exact amount of steps it will take to physically make it.  That way on your .idw sheets, you know the dimensions required for fabrication because those are the dimension you used to make the part

[mcgyvr]

There is a difference between learning Inventor and learning "design for manufacturability" or the skills and knowledge an Engineer or Designer should have about manufacturing processes and capabilities....

Haven't seen it but I assume the tutorial is just fine for learning Inventor... But as far as learning proper manufacturing/machining techniques,etc.. that part as modeled falls short.. And thats not what its supposed to be doing anyways.. Those that have responded here just know (based on our experience) that the part as modeled isn't correct.. But you would have NO idea and neither will the thousands of others before you that have followed that tutorial.. 

So don't stop watching the tutorials.. (but I'd think you've done plenty by now based on your previous posts.. )

Frankly I think you would have a better learning experience if you just grabbed something sitting next to you or around your house and tried to model it up..

Get a digital caliper and measure/recreate whatever is near you that you can get your hands on/take apart,etc...

The tutorial you are following seems to be the very basics.. I'm positive (I hope) you are way past that now.. So you are just doing the basics just to do the basics.. You already know the basics..move on to more... 

[SBix26]

@Anonymous I can't completely endorse your insistence on modeling exactly as the part will be fabricated.  That is sometimes a useful way to approach a taks, bu the process of design doesn't always work that way, and sometimes you may not even know for sure how your end part will be fabricated until it's nearly complete.

Of course, without taking fabrication into account you can end up modeling things that can't be fabricated cost-effectively.  But efficient and robust modeling doesn't necessarily mirror physical fabrication techniques exactly-- just as design parameters may be quite different from fabrication parameters.  I design a symmetric part around the center of the part, but I still draw it with dimensions from one corner wherever practical, because the needs of the designer are different from the needs of the fabricator.  That's the great thing about 3D modeling: you can have both: the design intent captured in the model, the manufacturing dimensions captured in the drawing.  Same with modeling techniques vs. fabrication techniques.

Sam B

Inventor Professional 2016 R3 SP2
Vault Basic 2016 SP1
Windows 7 Enterprise 64-bit, SP1

[Anonymous]

Again, thanks for replies!

:))

Can someone advise me on good tutorials?
Website with good tutorials?

:)))

It would be great if someone could devote some time to make a screen cast of how this valve should look in real life.

Several parts, assembly, constraints for assembly etc.

It would be benificial not only for me, but for the entire community 

Thanks!

[JDMather]

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s.shivaprem wrote: 

It would be great if someone could devote some time to make a screen cast of how this valve should look in real life.

Several parts, assembly, constraints for assembly etc....

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YYou should make this request to the author.