I wanted to let everyone know about a procedure I recently stumbled upon to create threads in a much easier manner. My pictures and suggestion relate to an external thread but I believe you can see it can be applied to virtually any style thread whether internal or external. In retrospect the application of this procedure doesn’t end with threads.

I’m sure your imagination will take you where you need to go to make your job easier using this process.

If your current parts are modeled with proper threads you can likely use them to simplify the process in adapting this method if you agree it can be used in your environment. You can use your existing threads to create a new tool.

I created the pictures and text below to do a presentation on Tips and Tricks at my SW (ConnSWUG) user group here in CT last night (6-15-2017) and it was well received, I hope you agree.

The picture below shows a 5/8-20 thread modeled in the usual circle-helix-sweep process. What I might do differently is that I do a full sweep cut of the thread profile at the end or left side in the picture. Then I do the rest of the process the same using a helix sweep cut. It does leave a clean 'manufacturable' end to the thread and this is actually done manually when cutting threads. Backwards to some but it's easier and lessens the chance of breaking the tip of the cutter. Of course you can also use a relief at the end, a swept cut perhaps .06-.09 wide to the minor diameter with some clearance. The threads may not be accurate but were only performed for a visual.

Here's a relatively standard 1/4-20 thread using the standard process. Note the 'ugly' end. Again the model may not be to exact standards.

I'm suggesting we create a tool to create the thread first and this part should be to the proper standards. This is a sectioned view of a 'tube' with a thread cut in it, both ends are chamfered as needed. This one happens to be 2.0" long.

I prepared a 'stub' for the purposes of testing the procedure.

Next using the Insert Part, Combine-Subtract method by inserting the 'tool' into the part needing threads.

Using the mates available, position the tool to 'cut' your thread. This one is set to create a 5/8" long thread.

And the end result. A nice (IMO) external thread at 5/8" long. I have the tool chamfers at 45 degrees, I would suggest the chamfer be half the thread profile but that's your choice.

I imagine you could save these tools as a library feature if you were to use a method such as this. You may also consider saving the dimensioned drawing view as a block to create future drawings as well.

I would like to state that in the example (1/4-20) the file size was almost 140K larger (831 KB- 693 KB) for the ‘combined’ part versus a standard swept cut version in 2014 and just 563 KB-316 KB in 2017. Perhaps SW could help in that by creating a process where we could save the end result without the overhead associated with processes such as this even if that removes the possibility of edits to the threads. Being this simple why not?

I’m hoping if this meets with your approval we can share our ‘tools’ somewhere. Any ideas or suggestions on this?