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Having trouble with Lofting,
paul_evans051
Member Posts: 4 ✭
I'm having two problems with Lofting so far, one where the thickness is an issue which is probably due to the other problem of not having enough points. I've tried to use the connections option in the tool dialog, to no great help. It starts with red bounds and when I try to fix those, more appear. When setting the thickness to 0.01", it works but of course this is not the desired thickness.
It was mentioned in other threads to set the thickness to 0.01 mm to try and troubleshoot the problem. I don't understand how that would help me troubleshoot though. In addition to that, it often leads to another problem or two: "Boolean operation results in non-manifold body" or something to do with merge scope, I don't remember.
I have two ideas on how to use loft, I wish to use Loft 1 using sketch 3 and 5, since that is the shape I desire. However I thought that using loft 2 with sketch 5 and 6 might yield better results because the two sketches ostensibly have the same number of points. However it also has red boundary issues, although it is certainly closer to the thickness I desire.
Answers
Your document is set to view only. It will help if you can set it to allow others to make a copy.
In certain cases where the error message is not helpful…Setting features to very thin tells you the loft can be made with your selected entities. And some tweaking or a different approach is needed depending on the problem.
I unchecked mid plane option. flipping the direction to fill to the inside will allow the loft to create. I also checked off trim ends options to make flat top/bottom cleaner look. not sure what the design intent is so this may or may not be a solution.
I suspect the mid plane option could of been creating some sort of self intersect or non manifold problems. If you need to use mid plane option. you might have to build it out in a few more steps starting this loft off as a surface instead.
Also when using mid plane… if you incrementally make it thicker from .01 to .02 to etc… when you get to .06" thick it indicates this red area as the problem area. So modifying your sketches may be necessary to resolve that area if you need to use the mid plane option.
I tried to share via the link with edit permissions, but I can't figure out how exactly. Besides that, since it's a public document I figured one could access it anyways.
Wow, I can't believe I just glossed over the flip direction. For some reason I also ran across the mid plane option as a troubleshooting step somewhere, I think. Thankfully I don't want it to be mid plane.
I forgot that continuing to work on the document would then change how people would see it after I've linked it here. Well, how then would I make the loft work for Loft 1? I still cannot get it to work.
In your loft 1 your are trying to loft a thin using edges and a face which doesn't work. you have to select edges and edges or face to face depending on the type of loft. Here's what I did to get it to work. you have to watch that sharp turn area as it will want to promote geometry that overlaps itself. 2 connection points that have to be held close together like the top profile help resolve this