Screw Thread Creation

[CorBlimeyLimey]

I've just been informed that SE can create threads in just "a few mouse clicks".

Is this true? If so;
Are the threads a true helical form?
How does it affect performance?
How often do you use that function?

 

[donyoung]

Hi,

Are the threads a true helical form?
- yes, use either helical cutout or helical protrusion
How does it affect performance?
- quite notable but that depends on the length and complexity
also the size of file will increase
How often do you use that function?
- never

dy

 

[donyoung]

/Edit

'never' in the meaning of: not to create threads

 

[Schipperus]

I think CorBLimeyLimey was informed that threads cen be created in Solid Edge in a few mouse clicks using the threads command...

This means the answers are:

No true helical form (why would you want it?)
It should affect performance a tiny little bit, but I've never felt any difference (the only thing Solid Edge does is remembering the thread and paint the surface green).
I don't often use the function, screws and bolts are taken from a library, threaded holes are made within the holes command.

As for how many clicks:

4, without options

IJsbrand Schipperus

 

[donyoung]

@IJsbrand,

that's right but the question was a bit ambigous and I've
seen (not quite often) models where the threads have been
cut using this function.
The thread function has no significant impact on the performance
the file size will increase a bit due to the fact that more
information has to be stored in the file.

dy

 

[CorBlimeyLimey]

Thanks for the replies, and my apologies for any ambiguity of my post.

In a thread in the SW forum, someone stated, "Making external threads in Solid Edge was a few mouse clicks, even to make tappered threads." I just wanted to have that confirmed or refuted. To compare, to create actual helical threads in SW we have to sweep a sketched profile along a helix. The helix and profile being created in separate sketches. SW has a Cosmetic Thread function which creates a dashed circle depicting the root/major dia of the thread and places a thread texture on the threaded surface.

So to clarify, does the thread command create actual threads, or just cosmetic (coloured or textured) ones, or both?

 

[donyoung]

Hi,

[cite]
So to clarify, does the thread command create actual threads, or just cosmetic (coloured or textured) ones, or both?
[...]

just cosmetic, either colored or as texture. For an inner
thread you will see the nominal diameter as dashed circle
the hole will be the core size (while placing the threaded hole)
The draft will show it then according to the choosen
standard (no further action required). To dimension it
you have to probably customize some settings.

dy

 

[CorBlimeyLimey]

Thank you.

 

[beachcomber]

And one other thing...
The thread colour on the part will be applied to the full extent of the cylinder to which it is applied, even if the thread is not defined the the whole way up.
It will, however, be depicted correctly in drawings.

bc

 

[donyoung]

Hi,

[cite]
he thread colour on the part will be applied to the full extent of the cylinder to which it is applied, even if the thread is not defined the the whole way up.
[/cite]

this has been correct in V20 but only for those threads that
are created in V20. Old parts are not corrected this way. This
new behaviour applies to internal and external threads.

dy

 

[beachcomber]

Thanks Don, I haven't really used V20 yet so wasn't aware that had changed.
I just started using it a couple of weeks ago doing some pipework stuff, but then packed my job in to take a bit of a break.

bc

 

[teebarr]

Hi CBL
I had a look at the original SW post and he is not talking about the thread tool which only applies a thread representation, but he is refering to the helical cutout tool which will produce a true helical form. He is correct in that this tool will produce any thread in about 4 clicks (once the profile has been established).
The workflow is simple:
1. Draw a sketch of a single thread (v or a simple circle for ball-screw)
2.Draw a line that will represent the axis of rotation as well as the thread extent (if desired).
3. Select the axis and the anchor point.
4. Select the pitch plus how you want to define the extent (extent or no. of turns etc. Additionally you can select LH or RH, taper, contant or ratio etc.)

I would use this to cut acme or ball-screw threads and can be useful for motion study. Also definitely adds autenticity to rendered drawings etc.

Performance does suffer if you have a lot of this stuff but I simply suppress the cutout until I need to use or see it.

HTH
Tony

 

[CorBlimeyLimey]

teebarr,
Thanks for the clarification.

 

[beachcomber]

teebar,
Instead of suppressing/unsuppressing the feature you could use 'simplify part'.

bc

 

[teebarr]

bc
I must give that a go - thanks
tony