Using English dims, convert to metric as needed...
Create the cylinder with an diameter that matches the Major Diameter of the
thread. Click (in WF2.0) insert, helical sweep, cut, bringing up the
helical sweep U.I. box. Select your attributes (default should be fine),
then click the sketching plane for the Sweep Profile. The Sweep Profile is
the path, start & finish, your cut will follow. Select a plane that cuts
through your cylinder length. Once in sketch mode, draw your Sweep right on
the diameter of your cylinder, from the start to the finish of your desired
thread location, then put in a centerline & complete the sketch.
At this point it will prompt you for the pitch of your thread, for example
20 TPI = .05 pitch. Once you input the pitch, your automatically in the
sketch mode to sketch your thread form. Sketch it your triangle (thread
form) with the "top" of the thread (between the crests) the length of your
pitch (.05 if 20 TPI), constraining it to the diameter of the cylinder at
the start of your desired thread location. Basic thread form should be
constrained 30 deg from the end of your cylinder, & 60 deg between the legs
of your triangle. Locate the top of your triangle .005 from the diameter
of the cylinder. Click done, & preview your threads.
If they don't work, keep hacking away, chances are there is something wrong
in your sketch, you'll get it.
Once you have created your threads, put a "starter thread", a 45 deg
revolved cut in, to
cut away the start of your thread.
Keep in mind your thread form will be .005 (or so) from the outside diameter
of the cylinder, leaving the O.D. to be the major diameter of the thread.
Once you have the threads working, redefine (edit definition) the feature, &
put in a .005-.010 truncation in the bottom of your thread form. At this
point you can locate the thread on the Pitch Diameter (or Effective Thread)
removing the .005 constraint, & also locate that truncation on the Minor
Diameter of the thread.
If this model is to be used in rapid prototyping of some sort, be sure to
locate the threads at the very lowest end of the P.D. Keep them loose is
what I am saying & they should work.
Good luck, this won't be easy to do without some real-time help.
regards,
Joe S.
Thanks a lot, but isnt there an easier way of creating an external
thread? I mean if I simply want to create a cylinder with an M12
external thread which i can screw into a M12 Thread Hole. There got to
be an easier way, right?
I Mean you can creat thread holes much easier. Why not external threads
which are in an ISO format.
Th
I take it you're new to modeling fasteners in a 3D CAD system.
While looking at the threads on a fastener doesn't give you chills
about the complexity, modeling them in CAD is far from trivial. There
is no automated command in Pro/E that makes screw threads accurately
and easily, and I'm not sure if any other major CAD systems do it
either. What Joe explained in such detail is how to make threads as
realistically as possible - which IME is only useful with making
threaded parts by Rapid Prototyping and for making photorealistic
models of components where showing the threads is very important.
In any case, realistic 3D threads are generally not desired. There is
no need to have the exact geometry of the threads in most cases, and
symbolic representation of the threads is usually enough. Even if it
were easy, screw threads can easily make the performance of an assembly
10x slower - and for no real benefit. Look into Pro/E's Cosmetic
Thread feature - it contains the thread information you're interested
in, it's visibly different from a solid surface (meaning that a rod
will look different from a threaded rod), and it will show on a drawing
with the standard hidden lines to represent the thread extents.
Dave
Thanks again, I'm really new in CAD modeling so any help is appreciated ;-)
I already used the cosmetic Thread feature but i was not sure if im
creating a thread hole with a specific diameter if i can fit my cosmetic
thread with the same diameter in this thread hole when generating an
assembly. Probably this question is stupid, since i can just change the
diameter of the external thread to fit in the hole. But since im
starting new i didnt want to model too complex or learn things which are
already incorrect so that my later model would be incompatible to any
assemblys or further constructions.
Thanks again
Yeah, stick with the cosmetic feature. I suggest making internal
threads with the hole diameter = inside dia of actual threads and the
cosmetic thread diameter = root diameter of actual threads. These will
display properly in a component drawing, too.
Then for fasteners do the opposite - make the solid cylinder = root
diameter of the threads and the cosmetic thread = the outside diameter
of the threads.
This way when you make the assembly you will not get any interferences,
and you can see if the cosmetic thread features align properly.
Dave
It's a very good, completely legitimate engineering question. I favor some
hole size with some fastener size and no interference. While I'm saying
this, realize that a few schemes fit this criteria. I favor the Pro/e
approach, embodied in the hole creation table: hole size is actually tap
drill size (not minor or root diameter of thread) while cosmetic is created
at nominal. With no interference, the fastener would be created at tap drill
size with cosmetic, also, at nominal... and no interference between solids.
The advantage of this method is that the tap drill size is saved in the .hol
files and is the foundation of the tapped hole. A constant reference which
your fastener must fit.
David Janes
Maybe I didn´t quite get that last one... but I´m still using 2001.
Now, question: has ProE eventually learned _not_ to interfere threaded
nuts´n´bolts in the mean time since 2001?
I´m using ProE´s "cosmetic" features for threads with _real_ values,
so drawings will be accurate enough for later drilling & milling...
Since V12 - when I learned to know it - ProE assumes interferences here,
which is quite annoying when looking for real ones in big assemblies.
And no way to mark some irrelevant - would be a good idea, wouldn´t it?
Oh, if only CAD system programmers had some basic engineering knowledge.
I´m sure such thing does exist even outside the metric universe ;-) ...
Walther
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