Newbie back, and dumber than ever (THREADS)

Okay... I've read and read, searched the group and read more, and even read your replies to my problem in the last thread I started,
and I *STILL* can't seem to grasp how exactly I need to make this happen.
I have modelled a part that is an extruded circle. Now I want to put external threads on it.
I have tried reading and doing, but cannot get it to work.
I have created a Helix of the right pitch, and laid it on the cylinder I extruded.
When I click on the Helix (selecting it) and then click "Swept Boss/Base", I get the sweep menu, but cannot get it to cut the thread. I get an error of - "A profile and path must be provided to define the sweep. The profile may have more than one countour profile for solid sweep/ To make a solid sweep, all the contours must also be closed. Sketch for profile and path cannot be pure construction geometry."
I can't seem to be able to select the "profile" part...
Is there some sort of online demo of this I can see?
This is kicking my ass.
Too, since I am not actually using this to mate with other parts and check for clearances, it seems that I am able to get away with "cosmetic threads" as many have recommended in other posts, but I'm so lame I can't even seem to get that far...
Help.
Best,
Weyland
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Weyland, Just out of curiosity, can you EXTRUDE the profile sketch? That's a good, quick check that your profile is 'one contour'. If you cannot even select it to be a profile, it smells like the sketch may not be a single close contour - if you also can't extrude it, you have your diagnosis that its broken somehow and needs to be fixed.
That said, you should NEVER! NEVER! NEVER! model accurate threads unless you will be machining (or otherwise creating a prototype) from the model or creating tooling from your model geometry. If you need it for visulaization or a rendering, try a displacemnt map or, if you must, fudge it with a series of revolves. Accurate threads take forevever for the modeller to build - though every new guy learns how to do it and invariably tries it, eventually every new guy learns it is dumb and unecessary (barring the exceptions in the first sentence of this paragraph)
Ed
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Ed,
Thanks for replying. More below.
snipped-for-privacy@juno.com wrote:

The part was created by affecting a revolve. You can see the gory details here - http://groups.google.com/group/comp.cad.solidworks/browse_frm/thread/7a0aeac425352eec/713d1e295b5fe9a0?q=weyland&rnum=1#713d1e295b5fe9a0

I have gathered that during my research, and am okay with that, actually. Sure, it would be good to know how and all that, but right now what I need are a few decent models and some drawings. *Eventually*, a proper model might be useful for importation into mastercam for actual machining, but to be honest, I'd probably rather just *DO* it in mastercam...
That said... what's a displacement map? I've created the helix, but it doesn't carry over when I create the drawing.
Best,
Weyland
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Weyland, I am not totally sure about this but from your original post I gather that you created the helix successfully, you never mentioned creating the profile sketch. I just want to double check that when you try to create the sweep you have TWO sketches, one is called the path and is your helix, the other is called the profile and is a completely separate sketch of something like a triangle, (that matches your thread profile for this case). Solidworks needs both to create a sweep. When first starting out with Solidworks it is often not obvious what the software needs given the rather criptic error messages.
Michael Dorman, CSWP
snipped-for-privacy@bellsouth.net wrote:

http://groups.google.com/group/comp.cad.solidworks/browse_frm/thread/7a0aeac425352eec/713d1e295b5fe9a0?q=weyland&rnum=1#713d1e295b5fe9a0
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See tutorial 4. Basically the same in SWX.
http://home.pct.edu/~jmather/content/CAD238/AutoCAD_2007_Tutorials.htm
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Or this http://www.mcadforums.com/forums/viewtopic.php?t937
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hey dear, After making the cylinder u want to make external thread for doing so you need 2 profile first heliex as path and 2nd thread profile and this thread profile must be drawn on the plane parpendicular to the helix curve at start point than Boss - Sweep the profile along the path hope it will solve ur problem.
and if u only want it fpr presentation than other option is insert - Annotation - Cosmetic thread.
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Weyland, I have created a step by step outline of the basic threading procedure, in the .doc format, made up of about 15 steps, that you are welcome to if you want it. It is designed to be understood by newbies such as ourselves. It is for a hex head bolt, with a cut SAE thread. Contact me snipped-for-privacy@deangelistool.com, if you have the need for it.
Good luck, G. De Angelis
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I feel your pain.....
I do threads a bit different...... forget the spiral. Draw a cross section of the thread. Copy it (or linear array it). Revolve it.
It isn't correct since there is no "pitch" associated but the threads look great and I can accurately dimension it for machining. Cross sections look great. Doesn't take too much memory. I can accurately fit parts together. My customers have never noticed.

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section
Array?!?!? Spoken like a true AutoCAD convert!! In deese heah' parts, wheeze call it a pattern! <just joking> ;)
Scott
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I'm on step 7 of 12.....

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So you want to put a plane perpendicular to the helix. Select your helix near the end you want to start from, then pick the plane icon on the Reference Geometry tool bar, or Insert/Reference Geometry/Plane, then pick Normal to Curve. Or you can start the plane first and then pick the helix.
Jerry Steiger Tripod Data Systems "take the garbage out, dear"
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Or it's even easier to select the helix and then select the sketch entity you want to create. SW will automatically create a sketch plane perpendicular to curves.
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I think that I had a similar problem one time which turned out to be an issue with the cut extrude. Apparently, part of the cut was off the end of the part, (the little corner)?
One solution could be to make the cylinder longer then it needs to be and then to move the cut plane up from the end slightly. Once this is done and the thread is cut, a simple cut extrude can be done on the end to make the thread the proper length.
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Yet another step saving move that I didn't know about.I owe you another beverage of choice, Matt!
Jerry Steiger Tripod Data Systems "take the garbage out, dear"
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Yea - what he said! :) You know, sometimes you forget to say the simpler things when you go by fuzzy memory....I see I also originally wrote "a plane 90 deg from your helix" - Kind of confusing rather than just saying perpendicular, huh? OK, well it was pretty early and I didn't have my second cup of coffee yet so I was typing with only one eye open. Anyone got any other excuse I can use?? (heh) I will refrain from posting before 8am from now on.... ;)
Scott

it
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