OK I'm stumped on this one today

[Scott]

Its a Boss-Sweep. I have the profile and the sweep helix path made. The
Profile has a Pierce Relationship to it and everything is just like the
other on that I made earlier....Now I get this Error when I try to sweep
them "Boss-Sweep3: Sweep operation failed to complete." Well no DUH!! If
Something is wrong I expect the Sweep to fail and be completed.

If it doesn't work Please tell what the problem is and don't give me
Information that I'm already aware of like....this Stupid Vague Ass Error
message.

See Here http://www.3dmca.com/Error_Messsage.jpg

Does anyone know what I'm saying here...and Can provide some reason or a fix
for this.....

Yes its a thread and Yes I know there are other ways of doing threads, but
this is the way I want it.

Thanks,
Scott

[Whit]

CLueless here, but is Sketch24 overlapping the helix paths?

signed,
clueless in Texas

[Edward T Eaton]

hard to say for sure, but it looks to me like the section might be wider
than the thread spacing. Sweeps can't cross into themselves, not even a
little bit.
If you must have the section wider than the thread spacing, you can always
sweep half of one turn, then sweep the other half of the turn, then pattern
those two features
Also worth mentioning...
its always better to have the sweep section outside the path - prevents
intermediate profiles from slamming into each other (I think that a sweep
along a spline is actually a loft behind the scenes, and profiles are
generated inside the modeler)
On a helix, just change the diameter so it is inside the section, and leave
the pitch and revolution count the same. You'll get the same number and
spacing of threads, but in a way that is less likely to cause problems.

On a simple sweep - one without guide curves - you do not need to pierce the
section to the path. That's one of those myths that somehow got out and is
widely accepted - but it is a myth (unless SW changed the code in one of the
service packs - they are mischievous buggers when it comes to sweeps and
lofts).

Cheers
-Ed

"Scott" <crede...@hotmail.com> wrote in message
news:alob71$1s3u4d$1...@ID-132888.news.dfncis.de...

[Scott]

Ya that maybe it! I'll check that out.

Thanks Ed

Scott

"Edward T Eaton" <ed'remove_this'17...@prodigy.net> wrote in message
news:FwRf9.766$AP3.30...@newssvr16.news.prodigy.com...

[kwbosch...@earthlink.net]

I usually try > Tools > Sketch Tools > Check Sketch for Feature, when something like that pops up.

Ken B.

[Steve Fye]

"Scott" <crede...@hotmail.com> wrote in message news:<alob71$1s3u4d$1...@ID-132888.news.dfncis.de>...

The problem is that you have way too many toolbars and buttons displayed.

Just kidding.

Steve

[Scott]

The problem was that the sketch was to big and was bossing into the other
revolution of the helix. Once I changed the sketch to a smaller value it
worked. I still don't see why that really wouldn't have the way I had it
before, but oh well.

If the Error Message would have read "Cannot make Feature, because the
feature extrudes into itself or something to the effect. I would have
understood my problem and fixed it, without having to post out here. Some
"Errors Messages" need more descriptive!

Thanks for the help guys!
Scott

"Edward T Eaton" <ed'remove_this'17...@prodigy.net> wrote in message
news:FwRf9.766$AP3.30...@newssvr16.news.prodigy.com...

[Scott]

"Steve Fye" <in...@rhapsodydesignsolutions.com> wrote in message
news:2e772407.0209...@posting.google.com...

LOL.....Steve!

Well when I run 1600x1200 Res. I have a lot of Real Estate so I place all
toolbars out when I start either a Part, Assembly or a drawing that way I
have everything available when and if I need it. Always be prepared for
anything ;-)!

Cheers,
Scott

[Whit]

Woohoo!!! I was right, woohoo.

signed,
Clueless in Texas

:o)

[Scott]

Thanks Whit and everyone for your replys and your help!!

Scott

"Whit" <whit@Texas_NO_POTTED_MEAT.com> wrote in message
news:3D8655F0.16AF348D@Texas_NO_POTTED_MEAT.com...