I am building a windmill blade and after creating planes, importing coordinates, converting and rotating when I try to loft these planes it doesn't get through. Can anyone please help me solve this issue.
Make sure your sketches are clean, meaning that they only have the elements in them that you want to loft together. Make sure the splines touch end to end with no gaps or overlaps. If you need reference geometry or other sketch elements, make sure that anything extra is turned to construction geometry. You can also use the Check Sketch For Feature tool, which will tell you if your sketch will work for a certain type of feature.
You might also turn on curvature combs for each sketch to make sure your splines don't have tight curvature. I'd also try to use the boundary feature instead of a loft and add a second connector to make sure the sketch points line up.
If you really want help, you need to upload a model.
Can you zoom in on the surrounding sketch of a green dot and show the screenshot?
There might be small entities and the order in which they are selected is not similar on every section.
Break each of your profiles into sections, and attached guide curves to them. You want at least 1 guide curve, and usually the more the better to get a desired shape. Without a guide curve the loft usually will twist.
Without guide curve
With guide curve
What you are saying has not been true for a long time. That and the "you have to have the same number of segments in each loft profile" claim. You can use connectors like guide curves, and they are created automatically. The blue or green dots in your screen shots are connectors you can use to straighten out a twist. And you can add a new set of connectors with a right mouse button click.
I never said you had to have the same number of segments on each profile, just to break them into sections so you have a point to attach the guide curve to. I find it way easier to use a guide curve then to mess with trying to move the connectors during the creation of the loft. My example was very simple and could have been done without the guide curve.
First, check everything that Matt Lombard stated. Then a good rule of thumb for lofting is that each profile has the same number of segments in it, check that. Next, right-click on the screen and select "Show All Connectors" and make sure that SOLIDWORKS hasn't selected the wrong points to connect one profile to the next.
And I second the "provide a file" comment as that will always get you a better and faster answer on the forum.
..for profiles like this (foils).. the culprit is at the trailing end.. that tail end (or the formula from which it came).. is usually closed.. with either a point of a extremely small curvature... and the loft guide at that end is too complex for the sections to cleanly transition between each.. it's direction typically inverts or are slightly askew.
If you can trim/cut away the tail so you have two endpoints or a sharp point (but be reasonable about making this.. not a sharp knife edge in reality).. it should resolve much cleaner.
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