thread run-out

[werks]

Hello out there. I designed a fastener in 3D with threads. The threads worked out great but now I'm stumped. How do I create the thread run-out? Does anyone have tips on how to achieve this? Even better would be a sample 3D model to show me how. Thanks.

 

[josephv]

Hello Wilton,

There is an shampoo bottle example from the Advanced Part Modeling course. They model the run-out by revolving the thread profile at the end of the thread. Your reseller should be able to email you the shampoo bottle.

If the run-out you modelled is somewhat complex, then a revolved feature may not be enough, you may need to create a swept profile at the end of the thread.

You may also want to look in the SolidWorks Model Library, there are a few examples of threads in there, although I could not find one with a run-out per se.

Cheers,

Joseph

 

[triggerguard1]

What type of fastener are you making? If you were making say a screw or bolt, you would need some relief under the head by means of a groove that would typically be made with a part-off tool. You can extend your threads past the groove, which will give a nice lead off of your threads, and make the model truely functional, not just hypothetical. If you're having problems with the lead on the end of the threads, set your helix plane about.100" off of the part face where the helix will lye. This will give you some clearance so that your thread profile sketch lies between the end of the helix, and the face of the part. Be sure to also dimension the thread profile from the end of the part to the tip of the profile. This will allow you to alter the extrusion distance or part length, and still retain the threads relative to the face.

 

[JNR]

A general comment and suggestion. WHY are you modelling threaded fasteners in detail? Hopefully because you really need to because we are actually manfacturing this special thread or making a special graphic presentation or some other GOOD reason? Standard threaded fasteners are rarely modelled in more detail than is absolutely necessary to get a space model and acceptable looking drawings. They are standard purchased items and most people just use a simplified profile with a boss revolve. Helixes are extremely slow (why the heck is that SW?). Once you get a few fasteners in an assemble with detail modelling in them you will grind to a halt computing trivial detail. At the very least have two configuration in each fastner model (cute and functional). Use the functional one until you need to plot and do a temporary switch. Same applies if you have lots of springs, etc.

3/4 of all the Spam produced goes to Hawaii - shame that's not true of SPAM also.......

 

[SBaugh]

I older versions of SW I could make this happen. But it looks like it has been fixed since then. Because now when I try it, it doesn't work.

JNR,

He maybe in a company like I used to be where they wanted detail out the ying wang. If that's the case then he will need to make detail threads.

But if he doesn't need too, then you "wilton" you should do like JNR says. Don't make them. Make fake threads by making a revolved cut and linear patterning it. If you need an example let me know and I'll upload one to my site.

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
When in doubt, always check the help

 

[werks]

Thanks to all for your suggestions & tips. We custom manufacture components with special threads. Any additional tips are welcomed. Thanks again. .

 

[SBaugh]

You could do it by making 2 helixes if you needed a thread runout. Example

1) You could make the body of the bolt
2) Produce the helix for the thread of the bolt. (Make the thread rev longer than you need too. see next operation to why)
3) When making your profile and offset it from the beginning of the helix. (Offset from where you start the cut-sweep of the profile so that doesn't start cutting for 1 revolution)
4) After the profile has been cut. Offset plane to where the thread stops.
5) Start a new sketch and make it so it runs off the part.
6) You can make it a helix if you need it to totally correct or you could leave it like it is, since it is a small amount.
7) Start a new profile sketch and do a 2nd cut-sweep.

If you need an example of this let me know and I'll make one and give you a link to it from my site.

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
When in doubt, always check the help

 

[triggerguard1]

That's interesting advice in regards to utilizing the pattern feature with a revolved cut. I haven't tried it yet, but I assumed that you wouldn't save anytime by doing it that way over creating it with cut sweep. I'll have to try that one out. I've been doing a lot of threads with the cut sweep method lately for marketing and patent purposes, but I may try this system instead if it is indeed faster.

 

[Timelord]

The methods suggested all seem rather complicated. SW 2003 will create a tapered helix (don't know about earlier versions). Make the threads with a straight helix and then create the runout with a outwardly tapered helix. Simple!

Timelord

 

[Timelord]

Wilton,

I just tested what I told you in the previous post (I was sure it would work, but just in case). Post your email and I will send you the file. (2.57 MB)

Timelord

 

[werks]

Hey Timelord & SBaugh. I'm anxious to try your suggestions. Thanks again to all; this is a very useful site and I'm definitely hooked.

 

[SBaugh]

http://www.scottjbaugh.com/Design_Portfolio/SW Models.htm

Here is a link to my site for a bolt made with 2 configs. One Config is with the above mentioned Runout and the other is with the fake threads, also mentioned above.

IHTH!

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
When in doubt, always check the help

 

[triggerguard1]

Cool SBaugh. Neat link. I hadn't considered the cut sweep with an arc for the path. I had only used a helix. I'll definitely remember that one.

Sometimes a guy just has to sit back in awe at what Solidworks can really accomplish. Thank god for the nerds. They really make life easy for me.

 

[werks]

Hey Scott, thanks for the link. I agree with Triggerguard1: you guys DO make life easier for the rest of us. By the way Timelord here's the email address where you can send your file: I'll definitely give it a shot. Again, thanks to all!!

tony@jordaneng.com

 

[triggerguard1]

Hey, I wasn't implying that these guys were the nerds. I was speaking of the programmers for Solidworks. Hell, If these guys are nerds, I'm one too, and man, I don't like the sound of that.
With any luck, this software will let me retire before I'm thirty. If that's being a nerd, I guess I'm all for it.

 

[werks]

Hey Triggerguard1,

I meant no disrespect. I just want to say thanks to all the talented people, including programmers, that make our life a little easier. Again, thanks to everyone and I really dig this site!!!

 

[JNR]

I figured perhaps you had a real need for this, but had to make the suggestion just in case.

Scott, glad you got away from the detail nerd that ruled your previous employer. Nothing ticks me off more than agruing with drafting managers for hours over "filled" arrowheads and crap like that. If it is good enough for ASME Y14.5 it is good enough unless there are specific extenuating circumstances!!

Anyhooo... simplification where appropriate can be a real time saver. For example We have a lot of heavily finned cast chassis. We have to model the fillets for good reasons. But by putting them folders and having a "speed" configuration with them suppressed really speeds things up for everyday use - specially when you have an entire aircraft installation open.

3/4 of all the Spam produced goes to Hawaii - shame that's not true of SPAM also.......