External Screw thread

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.

Bruin schrieb:

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