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?
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
snipped-for-privacy@yahoo.com.sg (John) wrote in news:559f7fc3.0407081201.4fa1ffb4 @posting.google.com:
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
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.
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.
If it doesn't take too much of your time. Could you please make the "loft the other direction" and send me ( snipped-for-privacy@yahoo.com.sg) 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:
In this fan
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"
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