complex loft

[j.j.d]

I am having difficulty lofting between these sketches. I need to constrain the loft to the shape in the top profile of picture four.jpg

I understand that I need to draw guides for the loft to follow.

In picture four if i try to loft to the next sketch It spits an error saying loft will produce self intersecting geometry.

Does anyone have any advice for me?

I can provide you with the sw part file (09) if necessary

-jjd

[j.j.d]

here is picture four

[j.j.d]

between each profile sketch must i have individual lofts because of the difference in shapes?

that is the only way i can loft the entire feature

[shift1313]

when you get the loft error, where does it say there is self intersecting geometry? the shape from the last drawing wont do you any good since it doesnt intersect all your profiles. You can loft without guides or rails but it really depends on what you need to end up with.

 

How many sections can you get in one loft without an error?

[j.j.d]

it gives the error when i press the checkmark to finish the loft. it is a rebuild error. see attached picture five.jpg

please note that the top outline sketch is just serving as a reference sketch.

in picture six.jpg the loft does some funny things between the 2nd and last sketches. am i correct to assume that i need rails or guides

 

thank you for your assistance

[shift1313]

I think you are going to need a few guides for that. try leaving the first(small profile) off the loft and see if you still get the error. I think because your second and third profiles are so close together, this is where your self intersection is coming from.

 

also open up your start/end constraints tab and play with the settings. you will be able to drive how your loft enters/exits your profiles which may help get rid of the issue.

 

Is it possible your sketch 20 has an error where it overlaps itself? can you make an extrusion with just that sketch?

[j.j.d]

do you have any clue as to what that error is caused by (picture seven.jpg)

i checked all the sketches and could find no errors.

is it possible that it fails because the number of lines/splines in each scetch differs?

[shift1313]

I think you are going to need a few guides for that. try leaving the first(small profile) off the loft and see if you still get the error. I think because your second and third profiles are so close together, this is where your self intersection is coming from.

 

also open up your start/end constraints tab and play with the settings. you will be able to drive how your loft enters/exits your profiles which may help get rid of the issue.

 

Is it possible your sketch 20 has an error where it overlaps itself? can you make an extrusion with just that sketch?

 

 

read above what i wrote. did you try this?

[shift1313]

if you are able to upload a SW file as a zip i can take a look at it some time today for you.

[shift1313]

ill take a look at it at work tomorrow morning. I would try using all the cross sections and try the start/end constraints to control the angle the loft enters each cross section. Whats happening without guides when your loft enters the second cross section its fine, but when it goes to the third the arc this makes is whats causing the issue. Ill let you know tomorrow what i find

[shift1313]

jjd, i got a little time to play with your loft this morning. The issue is the number of control points from sketch to sketch and the fact that these usually increase in the corner. For instance the first two sketches have 3 points in their bottom corners but the third sketch only has two. The self intersection comes when the loft tries go from lets say 10 control points down to 8 control points. i simplified your first few sections and this is the result(with no guides)

 

Others will know more about this but i would try to simplify things so each sketch has the same number of control points and try not to have them mid curve. When i was simplifying things a few of your sketchs would have say 3 straight lines on the bottom where 1 line would do.

[shift1313]

here is an example of removing some more points from the first sketch and adding 4 guide curves on the right side.