Sweep sketch fubar, another SW Corp screwup!

check it out,.. (originally created in July 2002)
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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!?!?!?!?!?!?!?!?!?
..
Reply to
zxys
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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
Reply to
John Layne
This is interesting Paul,
When Sketch1 is hidden, did you notice that the sweep fails/resolves/fails/resolves, like a toggle?
Muggs
Reply to
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 ___________ Muggs wrote:
Reply to
POH
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
Reply to
POH
I've sent it in to both SW Corp and the VAR. I doubt if I will get a SPR. I say that because, when I've sent in odd files like this is the past, NOTHING HAPPENS!!!! (and that maybe because the file itself is either corrupt or not repeatable for them to resolve and issue a SPR?) BTW, I opened it in SW2004sp5 and it seems to do a similar failure (not the same) so it may have started sometime during SW2004?
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"John Layne" Do you have a SPR number yet?
Reply to
Paul Salvador
Yep, it toggles. (fails/resolve/fail/resolve,..)
Reply to
Paul Salvador
Well, if you only close the open sketch and it will resolve the surface sweep. Hmm,.. it could be surface related, in that, the closed surface sweep boundary, like a solid sweep, removes the (open) variable in the calc for this to resolve?
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Reply to
Paul Salvador
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.
Reply to
kmaren24
..yep, and as you and most know, it should not matter. I and no user should have to workaround this error. I, you and most of us are not paying for workarounds. Or, is it, we are fixing things SW Corp breaks for us to workaround and pay for again, and again, and again,....
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Reply to
Paul Salvador
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.
Reply to
kmaren24
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
Reply to
John Layne
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.
Reply to
kmaren24
Ken,
Sorry but, no way, a sweep, especially this sweep does not need a constraint for the profile to the path for it to work. (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.)
Verification On, for me, has been on/off (usually problem parts) since I found out about it (1999?) and always on since the end of SW2003. And, verification on rebuild does "NOT" always catch rebuild errors as SW Corp leads you to believe. I've proven that verification on rebuilds is not a consistent option, if anything, it reduces your ROI for sure! But since about the end of SW2003 I have had it on all the time because of the excuses I've got (when they can't figure what is wrong) from SW and the VAR was with verification on!? Plus, I always ctrl-q, and that should show most problems/errors. IMHO, it's not what the problem is/was. There is something wrong with SW Corp and thier programming, period.
Your siding with SW Corp makes no sense.
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Reply to
Paul Salvador
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
Reply to
kmaren24
Best practices? Hmm, this "simple" sweep does "not" need a constraint (like a pierce or coincident) to work (that need was removed pre 2001). Yes, it shows some failure consistency in SW2004, 2005 and (I can't mention the next).
Something is wrong with SW programming, that's consistent.
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Reply to
Paul Salvador
Ken, Good practices? Why confuse the user? A point, in this case, is not a requirement for the profile to reference the path. Since this profile resides within the path (a closed profile) it should work (unless it overlapped itself). If the profile did not reside within the path, the profile would have to be moved or the path would have to be moved with the profiles starting plane. Otherwise, what you are suggesting, adding a point, is a workaround because the profile is laying on and within the closed path, SW, the program, is not working properly.
Sure, "if" I get a SPR, I'll post it to you and on the SW discusion forum.
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Reply to
Paul Salvador
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.
Reply to
kmaren24
Yep, that is what it says in the help but literary, a "point" is not needed. The path (a curve) must lie on (crosses over) the plane of the profile, that is the requirement.
What a "point" can do is help with any ambiguity (old issues, cya) but this is a simple analytical path it is sweeping on. The ill effects of adding a point is, it leaves a "seam" (at the start profile) on the surface, which is not desired.
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Reply to
Paul Salvador

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