SW2004 Loft Weirdness

Hello All,

Well as I'm wanting to see the "improvments" in SW2004, I thought that I
would try to recreate something I did some time ago. But, I'm getting a
weird problem when I create this loft: (SW 2004 Sorry)

http://home.comcast.net/~muggs828/solidworks/Port-1.zip

I created the exact same loft for an intake manifold using SW99, without a
problem, albiet without using a thin feature. I just shelled outward 4mm,
and that worked fine, in fact I'll add that as well.

http://home.comcast.net/~muggs828/solidworks/Port-2.zip

What is going on in SW2004 with the new loft (Port-1)? Maybe it's me.

Any ideas on how to avoid this would be appreciated,
Muggs

 

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"...

http://zxys.com/swparts/Port-loft-2003sp5.zip

Ahhh yes.... our subscription dollars at work....?????????????????????

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.

...

 

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

...

 

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

...

 

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.

http://www.frontiernet.net/~mlombard/Port-1m.zip

matt

 

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)

http://zxys.com/swparts/Port-1-loft-2004sp1-fitsplines.zip

We can workaround this for hours but it still is a issue of why? Why
did the loft fail? Why should the user have to repair it or workaround
the failure(s)?

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!?

...

 

But Daddy, I want a Umpa Lumpa loft!

... (too much willy wonka.) ;^)

 

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

 

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

matt.

 

Done, Thanks.

Muggs

 

Matt,

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!?

...

 

I need to do a better job at defining exactly

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

 

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.

"Edward T Eaton"

 

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 on geometry such as this manifold the only way one
could get even close to guaranteeing year to year repeatability is to throw
away the parametric model and replace it with IGES, STEP or parasolid.

Muggs wrote:

....snip...

 

Paul (and others),
You probably already know this, but it bears repeating. The loft algorithms
change every release, and sometimes between service packs. To keep data
safe, SolidWorks retains all of the old algorithms and uses those for legacy
data. In SW2004, if you edit a loft made in SW99 it will rebuild using the
SW99 algorithms. If you delete the loft in SW2004 and re-use all the
sections, guide curves (ick), etc. to remake the loft, SW will use the
present algorithms.
So, in theory, the loft can't change unless you delete it and remake it. In
practice, I'm sure that somebody (my bets on Paul Salvador because he's
really good at finding these things) has examples where the rules fail. But
that's how its supposed to work.
-Ed