Sweep sketch fubar, another SW Corp screwup!

check it out,.. (originally created in July 2002)

http://www.zxys.com/misc/sweep-failure-sw2005sp2.zip

Test, do a ctrl-q a few times and watch it fail!
Now, unhide sketch1 and ctrl-q, it resolves!?
Now, hide sketch1 and ctrl-q, it fails!?!?
Nice consistent program!?!?!?!?!?! POS!!!
Our subscription dollars going down the drain!!!

(btw, I created this in July 2002, and I never had
problems with it but now, I can see my subscription
dollars are really paying off!?!?!?!?!?!?!?!?!?

...

 

Very interesting, I'd like to see how SolidWorks responds to this one?
Do you have a SPR number yet?

John Layne
Solid Engineering Ltd

 

This is interesting Paul,

When Sketch1 is hidden, did you notice that the sweep
fails/resolves/fails/resolves, like a toggle?

Muggs

 

I've tried the CTRL-Q routine with BOTH sketches left hidden and also
find the rebuild alternately succeeds and fails - just like a
"toggle"...

It's the hiding of sketch 1 that promotes the failure, since the
visibility state of sketch 2 makes no difference.

This is truly bizaare behavior.

Per O. Hoel
___________

 

Here's an additional observation:

Paul's sweep is that of a surface. If the profile (sketch1) is closed,
the surface sweep deleted and the feature recreated as a solid base
sweep, then the CTRL-Q does NOT result in a rebuild failure - even when
the sketch is hidden.

There seems to be a glitch in the surfacing software?!

Per O. Hoel

 

I am sure this isn't something you want to hear but if you do a "what's
wrong" it says that the sweep section cannot find a point to start the
sweep ( I thought they fixed this) which makes some sense that the
sweep section lies in the middle of a line in the sweep path. If I
split the entity that the sweep section lies on and make that point
coincident with the center point that lies on the path it then takes
care of the "What's Wrong" message and gives is a point to start the
sweep. It then does not give the error. I had to make one more
relationship to fully define the sweep path and that was make the top
and bottom line symmetric about a centerline that was also added. If
anyone wants the part email me and I will send it.

Ken M.

 

I don't think it is a workaround in this case. Maybe the error could
have been that it should not have worked in 2003. Was verification on
rebuild there in 2003? The bug is that it should fail whether the
sketch is visable or not. Your sweep section lying in the middle of a
line is not a best practice. Move the sweep section to any end point
of the sweep path and there is no error. I have to side with
SolidWorks on this one. Sorry.

Ken M.

 

Ken, I can see your point, but it should be consistent. I tried turning
off verification on rebuild it didn't make a difference.

How about a situation where someone adds a lot of features, then CTRL
Q's and the model falls over?

The other day I was working with someone who had been using SolidWorks
for a couple of years (making simple prismatic parts), they didn't even
know that CTRL Q existed. Personally I rarely hit the Rebuild key any more.

John Layne <-- Not siding with SolidWorks on this one.
Solid Engineering Ltd

 

John,

I agree with you if best practices are used. I am not arguing a
general point of consistancy. I am specifically speaking of this one
part. Yes in general SolidWorks should be more consistant. This file
should not have worked in 2003. The fact that it didn't work in 2004
and now 2005 maybe shows some consistancy? For this specific file
SolidWorks isn't doing anything wrong. In general.....that's a
different story.

 

You're right a sweep doesn't need a endpoint or constraint. But it is
a better practice to.

Verification I agree stinks. I have better luck adding a new
configuration to a file to get the part to truly rebuild to find
problems than relying on verification. Verification for this specific
part does not matter since as Mr. Layne pointed out it doesn't make a
difference. (Verfication could be a whole new topic and the joke it is
for VAR's. It's my VAR's answer for everything. First question out of
their mouth is "Do you have varification....on?")

If you RC and select whats wrong in 2004 what does the error message
tell you?

"(I added a version in the zip which has no constraints, dims and the
path is on another plane and it still has the same problem, it should
not matter.) " Did you put a path endpoint on the sweep section?

If you just put a point of the path on a point of the section you don't
have a problem. Good practice.

Let me know if you get an SPR for this.

KM

 

snip it from help

Sweep Overview
Sweep creates a base, boss, cut, or surface by moving a profile
(section) along a path, according to these rules:

The profile must be closed for a base or boss sweep feature; the
profile may be open or closed for a surface sweep feature.

The path may be open or closed.

The path may be a set of sketched curves contained in one sketch, a
curve, or a set of model edges.

-->The start point of the path must lie on the plane of the profile.

Neither the section, the path, nor the resulting solid can be
self-intersecting.