# How to thread a cylinder in Solidworks?



## tino_ale (Jun 25, 2009)

Hi all,

Just trying to figure out *how to put some threads on a cylindrical surface in Solidworks*. What I want to do is very simple but I have found no simple function to do it.

Any tips?

I've found some methods describing how you should built a spyral, then define a triangle profile and remove material folowing the spiral, but I find it very troublesome for such a simple and common feature...

Thanks


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## precisionworks (Jun 25, 2009)

Draw the thread dimensions (as a triangle) & use "revolved cut" to to draw the thread - which will be a straight thread (not the actual helical thread that is cut by machining or rolling). A straight thread is good enough for most illustrative purposes, but if you need perfection, you'll need to generate a helix.

Only one triangle needs to be dimensioned, and then copy that however many times you need for the length of the thread.

Here are some different ways to it:

http://www.fcsuper.com/swblog/?p=139


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## PhotonFanatic (Jun 25, 2009)

tino_ale said:


> Hi all,
> 
> Just trying to figure out *how to put some threads on a cylindrical surface in Solidworks*. What I want to do is very simple but I have found no simple function to do it.
> 
> ...



There's usually no reason to actually model a thread--instead just apply a texture to visually show the thread in the model. You can spec the thread detail in the Cosmetic Thread feature.

For the extruded cylinder you apply a texture to show the thread, like this:







To apply the texture, do this:

Edit>Appearance>Texture>Thread>Thread 1 or 2

Go to Texture properties to set angle and distance

That uses a heck of lot less memory than the actual modeling would use, too.


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## gadget_lover (Jun 25, 2009)

I'm not an expert in CAD. 

I would suggest that in CAD, as well as in manual design, it helps to accurately dimension everything, especially grooves. Grooves can be decorative, for o rings or (when helical) threads.

Modeling the threads will help make sure that you do not end up with a cut-through or a part that breaks under minor stress.

Daniel


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## tino_ale (Jun 26, 2009)

Thanks for the advise.

What a bummer. I'm new to CAD and honestly, surprised such an advanced software can't model simple threads automatically from basic datas (TPI etc) :sick2:

Well I least I know what my options are.

I've been trying to model the threads with the helix+triangle method but could not succeed so far. I must be doing something wrong. I need to find a very detailled tutorial of each step, because I've spent so much time on this and I'm stuck!


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## PhotonFanatic (Jun 26, 2009)

Made using a Helix and a triangle. The trick is to be sure that the starting point of the helix is on the same plane as the drawing of the triangle. Then it is just a matter of creating a sweep.

SW is a PITA to learn and use, btw. :devil:


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## precisionworks (Jun 26, 2009)

> SW is a PITA to learn and use, btw.


And AutoCAD, and Photoshop, and ... every graphics or design program on the planet


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## Th232 (Jun 26, 2009)

precisionworks said:


> And AutoCAD, and Photoshop, and ... every graphics or design program on the planet



So true...

Although I've got to say, Autodesk Inventor seemed to be easier than most.

Or it could just mean that I've been using CAD programs for too long...


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## LukeA (Jun 26, 2009)

tino_ale said:


> Thanks for the advise.
> 
> What a bummer. I'm new to CAD and honestly, surprised such an advanced software can't model simple threads automatically from basic datas (TPI etc) :sick2:



Try Autodesk Inventor.


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## KowShak (Jun 26, 2009)

precisionworks said:


> And AutoCAD, and Photoshop, and ... every graphics or design program on the planet



Not every program.... just rather a lot of them.

Some years ago I found Rhinoceros to be easy to create basic geometry with, no doubt it will have changed in all recognition since I last used it. The package I worked on was called Workspace 5 and compared to some of the other CAD packages out there, it was very easy to model geometry with, the caveat is that it is a very specialist package and I don't think it has been developed or supported in any meaningful way for a few years. I found 3D Studio Max easy to model geometry in but again it's not a CAD package....


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## PEU (Jun 26, 2009)

There is no point in drawing the thread, instead what is used in solidworks are cosmetic threads, you define them, they appear in drawings and consume no resources.

Select an edge>Insert>Annotations>Cosmethic thread>blind then you select the diameter and depth and pronto! you can even add a callout with the details for the blueprint.


Pablo


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## tino_ale (Jun 26, 2009)

Ok I understant it's not mandatory or really needed to actually draw threads in SW, but I'm in the learning curve and for the sake of learning I want to succeed.

Well I'm stuck here :





I have my part.
I draw a plane couple mm under it.
I draw a circle, same axis and same diam. as the cylinder that needs to be threaded on the part.
I built a spiral as you see, starting from the plane and with some margin over the threaded portion. Starting 0° angle.
I built a triangle, then choose a point of the triangle and link it to the spiral.
I get out of sketch, select the triangle, and choose the "remove material" function that can follow a path.
The triangle is already set as the "profile". I choose the spiral as the path. Click "Ok" and get an error message like : "the operation has not finished".

What am I doing wrong? This thing is driving me nutssssssssssss


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## PEU (Jun 26, 2009)

here you go: http://peu.net/temp/screw.zip 

the feature used is a swept cut.


Pablo


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## McGizmo (Jun 26, 2009)

In the old SW99 that I have and use, I had "fun" cutting a thread as well and found that the feature was too demanding on the software to bother with. I can't recall the terms but I had to set the helix path with the triangle so that it "pierced" the triangle or something like that. I also found that my triangle needed to extent past the material being removed as I recall. I wonder if you would have success if you enlarged your triangle beyond the cylinder.

In practice, all I do is put a 30 degree chamfer on the leading and trailing edge of the part with minor diameter being that of the intended thread's minor diameter. In many cases, it's a chamfer at the end of the part and a 60 degree groove inboard representing where the thread ends.


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## PhotonFanatic (Jun 26, 2009)

tino_ale said:


> Ok I understant it's not mandatory or really needed to actually draw threads in SW, but I'm in the learning curve and for the sake of learning I want to succeed.
> 
> Well I'm stuck here :
> 
> ...



You have the sketch on a plane that is different than the plane of the starting point of the helix. If you set the starting angle of the helix to zero degress, then you should draw the sketch on the Top plane. 

If you draw the sketch so that the starting point of the helix is within the sketch, then all you will need to do is to exit the sketch, then choose Insert>Cut>Sweep and choose the sketch and the helix in the respective boxes, then click OK.

You should get this, although you may have to dimension the outside of the triangle so that it is just outside the diameter of the area you want threaded:






And, of course, once you manage to do this, someone will come along and ask to see a different pitch on the threads. :devil:


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## tino_ale (Jun 27, 2009)

Guys after many hours I have finally succeeded :sick2:

Why I had problems : I still don't understand why!!  My triangle sketch was on the same plane as the starting point of the helix. I followed a tutorial, could still not succeed.

Heck my problem could be a bug of SW? I don't know.

Anyway. I noticed on Pablo's screw that the triangle was "loose" with no connection or precise dimensions, and it seemed to work.

So I came back to my triangle sketch, erased it and made a new approx one. It WORKED.
Added a "link" to the spiral so it's outer edge would line up with the surface : it WORKED (it doesn't seem to need to extend beyond the part,a t least in my SW).
Added all the details on the triangle (60° angle, depth of cut...) : did NOT work all the time!

Depending on the size of the cut, the sweep cut cannot succeed. Right now it works but if I increase the depth too much it can't rebuilt. I could not determine, yet, what exactly is the problem. I suspect it becomes problematic when the path of the triangle along the helix will cut the same material more than once in the operation. But I'm unsure.

Anyway, THANKS all of you for helping. Got my part done  

I don't have my SW environement now but will post pics later on...


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## kuksul08 (Jun 27, 2009)

They don't usually use the extruded threads like that unless it's purely for aesthetics. Solidworks is actually a very intuitive program and extremely useful. I am trying to learn ProE right now but it can be more difficult.
Anyway, unless you are just showing someone or having it SLA'd I would just use a thread call out instead.


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