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How to create blended thread end


Hi Guys
we used to create a thread end like this in proe is rotational blend command. But how I make it in Catia I am sharing with you and need your opinion as well as another approaches.

just create a shaft feature of any dia and make a sketch on yz plane like below on diameter surface. this is for starting point of helix.

Now go to generative shape design and create a helix on lower point of sketch2. My perameters are 4 mm pitch and 20 mm height (5 full turns).

now create a sketch on yz plane and lower point of sketch2 or start point of helix. triangle is for thread profile and left portion is to close the thread section properly.

Edited by: Zaki


Now go back to part design workbench and create a rib using sketch3 and helix1 as center curve.

its your basic thread and now you need two portions of thread that blend that makes it real looking thread (specially on plastic bottles). Now create another helix on upper end point of helix one. same pitch and 0.5 mm height (just a 1/8 turn of a thread).
Note: use Z axis as helix axis always in this tutorial (right click on axis tab and select z axis from contextual menu).

Now you need a spline from upper end point of thread to end point of helix2, tangent to threads edge . reverse the tangent direction if its going wrong.

now you need a section same like thread section on the end of thread. so create a skecth on upper end of thread. Its perallal to yz plane in this tutorial.

now create a rib feature in Part design wb. use sketch4 as profile and spline1 as center curve. Ignore the warning.


Its looking like this.

Now you can create another end by same technique.
Please let me know if you guys use another approach for this process.

Edited by: Zaki


New member
Hi Zaki,

This is the way everybody is doin it :D

I couldn't notice that also on the on the CCV challenge you don't fully constrain your
Use the ("traffic light") Sketch Solving Status button on the bottom of the screen when you are in sketch and if the result is Iso Constrain is ok, if is under constrain look for the orange points and lines.

The second method is to go in tools, Parametrization Analysis and from the combo box select Under-constrain Sketches. If a sketch name will appear this means that the sketch is not fully constrain.

When u use wireframe geometry (points, lines, planes, etc) after you apply surface based features you can also use "Delete useless elemets" so you can get rid of the elements that you dont use.


Hi Hardy,
Actually dear we use rotational blend in ProE and its too easy command. But I was consios about Catia and make tries. Suddenly I got the helix idea. Because helix is not easy in pro. And I got it. I shared it here because most people says that catia guys dont share thier knowledge. Thanks for your comments as I am in learning phase till now man. I know I left a lot of things in Fan but It was just fun to learn and know about as many features of catia as possible.


Hardy dear! how can I save my R17 part compatible to R16? I saw a thread in V5forum, but I cant get it today.


New member
tools -> Utility -> DownwardCompatibility

But will be without history

If you need history then you have to redesign in R16 (to make your work easier use Feature recognition for simple shapes)


New member

Thanks for sharing your solution for the plastic bottle threads. Using 3 helixes is a good, easy to understand method.

One suggestion: make the 3 helix curves and join them first, and then you only need one rib.

Another alternative -use a fillet to round-off thethread ends:Since this is a plastic bottle and the thread profileis not sharp, use a trapazoid for the thread profile, and make a single, constant radiushelix the entire length of the thread. Make the rib with the trapazoid. Use a fillet to round off the edges at both ends. Add a Tri-tangent fillet to round-off the flat on the thread.(I find this works best if the thread is in it's own partbody)

Edited by: nappie


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