Plz help, computer fan blade loft feature failed.

Greetings:

I wish to re-trace the steps of creating a computer fan (file download
from 3Dcontentcenter site). I create 3 sketches (#5, #9, #10) on the
hub. Then use a loft feature, selecting Sketch #5, 9, 10
respectively. After hitting the green check mark, I receive this
message:

Loft: Cannot knit sheets together.

Note: I did try to select the sketch in different order and still get
the same message.

Does anyone have an idea what I am missing here?

http://home.comcast.net/~wangphk/SolidWorks/Parts/Loft-Feature-Failed.jpg

 

possibly you need to add a couple of connectors along the bottom of the loft
to clarify the loft going from a three sided profile to a four sided one

 

It's hard to tell what's going wrong from the picture, but my first guess
would be that your connectors are crossed. each sketch has 4 segments, but
on two of the sketches, there are very short lines. the connector handles
show which end of what line is connected where. you'd have to zoom in on
both of the pointy ends to see if the connectors cross themselves. You can
also RMB in the view when editing the loft and select "show all
connectors".

aside from that, you might try lofting as a surface and see if the error
still exists. you might also try lofting individual sketch segments using
contour selection.

are you using any end conditions like tangency or direction vector on the
loft? if so, turn them off. also, just to force it to do what you are
asking, you might try a couple guide curves.

it looks like part of the problem might be that the profiles are at such
steep angles to the shape you're trying to create. Ed E would be able to
articulate this better. Just because you downloaded something from the
SolidWorks website doesn't mean that it shows good techniques. This is
definitely a goofy loft. I downloaded the part you're following, and I
wouldn't approach it that way, (not that what I'd do matters). I would
probably loft the other direction, which would be a more complex set up,
but is more likely to produce better results, especially on the leading and
trailing edges of the blade.

matt


(John) wrote in @posting.google.com:

 

aside from that, you might try lofting as a surface and see if the error

First, each loft is its own animal. If anything I write below sounds mealy
mouthed - it is. There are so many little issues that could be behind this
that I cannot be definitive without having the part myself.

I like matts suggestion of lofting the individual 'sheets', though I have to
admit I am novice to the contour selection part of it (I gave up on contour
selection after my first few ugly problems with it). I usually do what
needs to be done by converting entities into new sketches.

About the knitting sheets together error - Solid lofts are a little program
(like a macro) that automatically creates a bunch of surface lofts. What a
solid loft does is it lofts each face one at a time from your profile -
these individual surfaces are for some reason called sheets (why they are
not called faces or surfaces in the error message is beyond me). Then the
sheets are connected (knit) to enclose a volume, which then gets defined as
a solid.
When SWx cannot 'knit the sheets together' that means the sheets overlap,
intersect, or pull away from one another - basically, some condition exists
that will not allow the indidual surface to be stitched into a single closed
volume. What will cause this? Frankly, sometimes SWx just sucks, the loft
is not behaving as it should and there is nothing you can do about it.
Sometimes its because your loft section placement adds too much 'pressure'
to the loft (which seems to me to be the case with your loft), but we would
have to go into a lot more stuff to talk through that bit of business.

If you were to loft the sheets individually or in smaller groups yourself as
individual surface lofts instead of having SWx loft all the sheets at once
as a solid, you would probably get to see where the problem is. You then
might be able to add some guide curves to help eliminate the overlap,
intersection, or gaps that are causing the knitting problems. Sure, guide
curves add pressure and problems of their own, but they look like they may
be appropriate in this case (but don't think you will get off lightly - my
guess is you will need one for each of the four corners)

The preview of your loft in the last image sure takes an ugly turn where it
starts on the left side. According to the group boxes in the PM it is not
due to a start or end direction or tangency condition, though matts
suggestion is what I would have guessed had the PM not been shown.
It would be useful to see how the angles of the profiles work - profile
angle can add 'pressure' that kill a loft. To learn about pressure, get in
the habit of looking at the 'face curves' (see the hlep) of lofts you make
to get a sense of what happens to the UV lines of a face based on these
things that influence their pressure. You will see strange jogs, kinks,
convergences in the face curves, and you can then amalize your model to
figure out what causes the imperfections.

Based on that shaded preview, you really ought to try to add two guide
curves on the 'hub' end of the loft. The guide curves are easy - use 2
curves through reference point or sketch splines in two 3D sketches (the
same thing, when you strip away the 'macro' junk) that connects the
appropriate 3 points of the 3 profiles. This will clamp out any tendency
for those faces to cross.

I wish! I hate talking about lofts because it is such a subtle, situational
art.

Just because you downloaded something from the

 

Thank you all for your detail analyzing and help.

------------------------
Neil:

All the sections are 4 sided. It could appears to be 3 since the side
could be so small about 0.5mm to show in the picture. I am unable to
add more connectors, since SW has been taking care all of them.

------------------------

Matt:

The short line from the 2 sketches (Sketch #5 & Sketch#10) you're
referring to is a little arc.

When closing-up on the connector, I don't see they're crossing
themselves
http://home.comcast.net/~wangphk/SolidWorks/Parts/Loft-All-Connector.jpg

Did you download the 120mm Irwin (the very first / top file) model
from the 3Dcontentcenter? If so, could you please delete the loft and
try to redo it using the same sketch. I try and have the same result.
Am I missing something?

<<aside from that, you might try lofting as a surface and see if the
error
still exists. you might also try lofting individual sketch segments
using
contour selection.>>

Surface loft is working. I have to surfaces instead of a solid.

Contour selection or not, selecting any two sketches in any order, it
works. Adding the 3rd sketch fail.

<<are you using any end conditions like tangency or direction vector
on the
loft? if so, turn them off. also, just to force it to do what you
are
asking, you might try a couple guide curves.>>

No I do not use any end conditions. I just try to keep it as simple
as possible.

As far a guide curve, it isn't a cakewalk when sketching a 3D guide
sketch, especially in this case though. I would be much interested
to learn how to create a guide curve in this particular case.

<<...Ed E would be able to
articulate this better. Just because you downloaded something from
the
SolidWorks website doesn't mean that it shows good techniques. This
is
definitely a goofy loft. I downloaded the part you're following, and
I
wouldn't approach it that way, (not that what I'd do matters). I
would
probably loft the other direction, which would be a more complex set
up,
but is more likely to produce better results, especially on the
leading and
trailing edges of the blade.>>

If it doesn't take too much of your time. Could you please make the
"loft the other direction" and send me () the
file so I can take a look at your technic?

---------------------
Ed E:

Thank you so much for taking your time and explain clearly what is
going on with SW loft feature.
If you don't mind could you please d/l the 120mm Irwin fan from the
3DContentCentral. It's the 1st one under User
Library/Electrical/Fans. As I mention earlier, once you delete the
loft. You will be unable to redo this feature.

---------------------

 

It didn't occur to me that the part had been built already in SWx.

The loft fails because of a regression bug. Loft features continue to use
the algorithm from the version in which they were first created. Deleting
and recreating the feature causes SWx to use the latest algorithm. Some
sort of regression has occurred in the altest algorithm, and the feature no
longer executes.

I will submit the bug through our VAR. You should consider doing the same.



By the way, it takes about 1 minute to throw in the guide curves, and they
save the feature. You really only need one to keep the feature from
failing, but adding one introduces pressure to the loft that effects all of
the other edges. Just to keep things tidy, I went ahead and made four.
Pretty simple problem, really.

 

Ed E:

Thank you for the attach file. I see now. I just need to create a 3D
sketch that connect the corner of the profiles all together.

Can you recommend a general technic that will guarantee the success of
a loft feature? What I mean is as a general practice should I create
more guide (at least two) curves for the loft feature? In this fan
case it was easy to create a 3D sketch to connect the endpoints of
profiles together. However, what would happen in a case such as
circle, ellipse, close spline...where the profile doesn't have
endpoints.

Thanks for everything.

 

Ed E:

Thank you for the attach file. I see now. I just need to create a 3D
sketch that connect the corner of the profiles all together.

Can you recommend a general technic that will guarantee the success of
a loft feature? What I mean is as a general practice should I create
more guide (at least two) curves for the loft feature? In this fan
case it was easy to create a 3D sketch to connect the endpoints of
profiles together. However, what would happen in a case such as
circle, ellipse, close spline...where the profile doesn't have
endpoints.

Thanks for everything.

 

Ed is such a nice guy he will probably answer you, but I will jump in
anyway. There is no hope of ever coming up with a general technique for
successful lofting. What works and doesn't work changes from SP to SP. This
is one of the really painful parts of SW to deal with.

Sometimes guide curves help, as in these fan blades. Other times they hurt.
My general rule (even though there are no general rules) is never to use a
guide curve unless you absolutely have to. Work your way through Ed's Curvy
Stuff tutorials on the DiMonte Group website:

http://www.dimontegroup.com/

You can put points on the curve, then mate them to the sketch, or you can
use construction lines that cross the curve and mate to both the lines and
the curve.

Yes, Ed, thanks for everything!


Jerry Steiger
Tripod Data Systems
"take the garbage out, dear"