SW2004 Loft Weirdness

if you move your connector to the bottom it looks much better

actually I see I had it placed diagonally when I said that - guess you have to play around with it a bit

LOL ....ignore my posts Muggs... I am having a really bad day!

Muggs,

Yep, consistency with lofts and sweeps are a joke. Consistently inconsistent should be SW Corps motto. (here that competition!? you can nail them on this issue!)

Here is a SW2003sp5 file of a single port to isolate you from it being "your problem file"...

A Parasolid or SW Corp problem,... any bets!???

Anyhow, thanks for posting it. I see problems all the time with my files and other user files. Oh btw this is a solid problem, so for you who think this is a surface issue... it's NOT.

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Muggs wrote:

Nah, it's a SW Corp consistent inconsistent consistency.

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neil wrote:

i.e.,.. it's both a solid and surface issue, one in the same.

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"Muggs" wrote in news:ucGdnTUIo snipped-for-privacy@comcast.com:

If you create a fit spline on both profiles, the problem goes away. You should also use the advanced smoothing switch to join all the faces together. Your original uses maintain tangency, but if you have closed splines for profiles, you don't need that.

Also, using the slider in the centerline parameters to turn down the number of profiles smoothes it out a little so it doesn't have such nasty tight spots. It looked best when I pushed it all the way to the left, which made 13 profiles. All the way to the right makes 120 and a couple very pronounced nasty spots.

Weird problem to be sure. I tried to break it down to see exactly where the problem is. If you just loft the end arc of Sketch5 to the short end line of Intake Port 1, (using a lofted surface and changing the rest of the profile to construction geometry), it does the transition just fine, but if you add an adjacent short arc to both profiles it seems to completely ignore the centerline, and doesn't look anything like the problem you were seeing.

I also tested it by taking your old part, and deleting and recreating the loft. Same problem. I tried getting rid of the coradial sketch relation and replacing with a tangent, same thing. Same thing also if you make the centerline a 3D sketch spline instead of projected lines and arcs.

Have you sent this in yet?

Anyway, here is a link to the part using the things I talked about. Hope it helps.

That's weird allright. In fact, that's the exact type of problem Autodesk Inventor has suffered from (not sure if it does now).

What... does SolidWorks use ACIS now for new lofts ;^)

Even if I open your Port-2 part, erase the loft, and re-create it, I get that same bulging.

If you edit the definition of the loft, RMB in the graphics area and select "Show All Connectors" you can sort of tweak things until they work.

If it were me doing this, I would most likely add another profile somewhere to define the shape a little more. I'm thinking you might be relying on the software too much and it's trying it's best to 'guess' what your design intent is.

This is a great example of why some of us complain so vocally at times. This inconsistency really deserves an explanation.

Now where are my French Cries and Whaaamburger. (Oh yeah, and a Whiiiineken).

Mike Wilson

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Yeah, but using fitsplines causes another problem using the original sketch, the loft results in split isoparms as well as a different loft..(not good)

BTW, this is not directed at you, Matt. We all know you are trying to help.

But, SW Corp needs to answer this question!? So, why SW Corp!?

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matt wrote:

But Daddy, I want a Umpa Lumpa loft!

.. (too much willy w>

Paul Salvador wrote in news: snipped-for-privacy@verizon.net:

That's why I said to use the Advanced Smoothing switch, which gets rid of the segmented faces. If you use that switch on the model you posted, it looks ok (actually it fails, but it works if you use the setting when the feature is originally created instead of changed as an edit). His original loft used the Maintain Tangency, which keeps the face from segmenting when the profile is lines and arcs.

You're right it's a somewhat different loft because of the difference between the spline and the lines/arcs, but in the fit spline dialog you can control how much it will deviate. Plus, from the looks of things, if he was just using a centerline loft, he wasn't too concerned with tight control.

The guy asked for a workaround, and I provided one. That was a question that could be answered. I don't think we can (or SW will) answer the other questions, and even if they did, I don't think the answer would be of any use to anyone.

matt

OK Matt, Thanks,

I used Fit-Splines, and that helped some, then I moved the Center line parameters slider all the way over to left, and that looks even better.

BUT, Paul I completely agree that Lofting (and everything else for that matter) should get better with each release not worse. Mike, I also completely agree, I need to do a better job at defining exactly what it is I want the loft to look like by 2 or maybe even 4 guide curves.

Also, should I send this to SW? And should I send it directly or though my VAR?

Thanks again for your help, Muggs

"Muggs" wrote in news: snipped-for-privacy@comcast.com:

Send it to your VAR. That's how things get fixed.

matt.

Done, Thanks.

Muggs

Yep,.. it fails but this brings up another issue,.. why does the loft edit retain past settings during the edit, why aren't the cleared during the edit? Even doing a few test with Muggs part, I would also have sketches which would be absorbed into the loft but not shown in the edit list,.. it's flaky. Or why can't a user re-use or share a composite curve or why can it be visible but you can not select it?? The user has to start over again or sabotage the data to workaround these inconsistencies.. not at all productive.

True but parametric consistency is the issue, it's inconsistent,.. that is a problem, time is lost, productivity is lost...

Yeah, I understand that and I'm definitely taking advantage if this and highlighting this issue because it is a on going issue and I'm tired of seeing it. ...ah, but that means more free help from the SW paying beta testers!?

There is no black magic about solid/surface modelers so the answer to this question is important. The users should understand why this is happening, why the tools are failing and why they have to workaround these problems and lose time because of these inconsistencies.

So, SW Corp or whoever you programmers are,.... What's the deal!?

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FYI - You can't use guide curves with a centerline loft

I enjoyed looking at your part. Boy is there a lot of stuff to dicuss about it... I only have a minute, so here's a couple of things that might be useful:

-The 'curvature' of your centerline will influence the twist of the itntermediate sections. To see this, convert your projected curve into a 3d sketch, and RMB click-'show curvature' on the segments. The curvature combs will stick out of the spline like a dorsal fan on a lizard. The intemediate sections will try to twist to maintain the same orientation to the 'dorsal fin' as the first section. This curve would require a lot of care to execute in 3-d with control - you will likely get crazy twisting. Just changing the centerline to use the planar skech CL front, edited to be on a plane that interseects both your profiles, gives a much better looking loft.

-A loft executes one sheet at a time. Even though the sections are tangent, the loft doesn't care - it pretty much deals with each sheet as its own, screw the connection. Learn this, and you will start to get things under control

-I think my brain's been changed by my years using SWx. I just naturally look at soomething like this and think 'of course the body of the loft is messed up - you have provided almost no information'. You've created a beginning, an end, a path, and told SW to do its best. SW is a mindless program - it is really unlikely that its going to guess right. I would try to break this loft into three sections so I could really be in charge. I would do the pellet shaped end of the manifold as a seperate loft or revolve, and the other end of the loft (probably) as a simple body (extrude in one direction, cut in the other, then filet) just to keep it simple. Then I would loft between them with start and end tangency. The reason to get the ends in first it to make sure the loft is heading the right direcion before going through the tough transition. Its a little bit of work, but you'll get what you really want, and eliminate problems that arise from SW being dumb.

-Barring that, add a couple of sections. Better yet, add a bunch of sections and get rid of the centerline, using it only for construcion. You are having problems because SW is creating a bunch of sections for you automatically, but its stupid. You can make those sections yourself, and you are smart.

Gotta go - good luck

-Ed

news:ucGdnTUIo snipped-for-privacy@comcast.com:

One other thing that got stuck in my brain... I have no idea what manufacturing process you will be using to make this part. I'm concerned because I really don't see any consideration for manufacturing process in the loft itself. If it were sand cast, for instance, you would have to be putting parting line and draft information into this thing. I assume that the consumed piece in investment casting has the same concern (even though it is consumed, you have to make a bunch of them, right? I've never been involved with investment casting myself, so I admit my conjecture)

You can paint yourself into a corner if you use loft constructions like this. SolidWorks is using the centerline and some internal logic to orient a lot of extra loft profiles, none of which know or care about your manufacturing concerns. Each of those profiles is sort of averaged from the ones you provide, which again causes problems since drat and whatnot aren't accounted for.

Its really neat to get weird shapes with very little setup. The problem comes in when we rely heavily on those weird shapes, mostly generated by the computer, then have to go back and be designers after the fact. Be the designer up front, set up the loft with lots of intelligence and control, and you will (almost!) always come out OK.

I suspect you were making a concept model, so the above may not apply. But if you are going into production with this thing, it pays to put the detail in from the beginning.

Thanks Ed for your insite.

Actually this port is part of an intake manifold that I did for a company called PES about 4 years ago now. It was sand cast, and the parts are now in production, and with an Eaton (any relation?) Supercharger mounted on top, it makes BIG power.

Also, in referance to your last post, I was going to use 2 or 4 guide curves instead of a center line loft, I realize that I can't use them together.

So, having said all that, I may have to make another (different) one, and any thoughts that you have on how to improve my lofting capabilities would be very much appreciated.

Muggs

Muggs,

This is kind of scary to hear. When using lofts how can one be certain that a part made on one release is going to be the same part two or three releases down the road?

It would seem to me that ...snip...