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Having trouble with a loft/sweep function and cannot figure it out.

Hi All!

I'm looking to sweep or loft this profile but it keeps giving me an error. I'm using the faces of sketches 16 and 17 as the profiles and sketch 18 as the guide. I teach CAD at a HS in NJ and one of my students is trying to replicate the item in this link. http://www.agcross.com/wp-content/uploads/2015/08/buildup-3.jpg

This is what it should look like: http://www.agcross.com/wp-content/uploads/2015/08/buildup-4-585x444.jpg

Thanks for the help in advance!

Answers

  • shane_evans075shane_evans075 Member Posts: 4
    I uploaded the file as public. It's called CLUG loft issue
  • jakeramsleyjakeramsley Member, Moderator, Onshape Employees, Developers Posts: 584
    Guides need to exactly touch the profiles that are being used and are only done locally.  This loft has two issues:

    1)  The guide (sketch 18) doesn't touch the end profile (sketch 16) correctly.  I updated sketch 16 by removing the two external points


    I then saw that the vertical line was off of the face of the edge.  I had to delete the projection constraint on the bottom point.  I then made the bottom point piercing with the bottom edge.  This forced it to be on that face.


    I then opened up sketch 18, the guide and saw that the end to sketch 16 wasn't fully constrained.  I grabbed it and moved it around which meant it wasn't on the vertex


    I selected these two points and made sure they were coincident.  This forced the guide to go from one profile to the other.


    2) as the guides are just local, the other vertices try to do a shortest distance to corresponding vertex.  As the profiles are 90 degrees apart, the default will cause the loft to twist on itself and fail.  The loft needs more guides.  I noticed that the size of it doesn't offset great as the nice curve on the edge becomes 0 radius resulting in a sharp right angle which might look weird.



    Look at this, the start and end profiles look roughly the same.  If they are intended to be the same, I would suggest doing a sweep instead of a loft.  They are far more forgiving for the paths compared to the guides and only need one end profile.  If not, then I would suggest fixing the profile in sketch 16, update the guide in sketch 18 and add guides for the top two points.  On thing that may help going forward is to use the sketch split command where these sketch curves meet to give a vertex to attach a guide to (and create sketch planes on).
    Jake Ramsley

    Director of Quality Engineering              onshape.com
  • shane_evans075shane_evans075 Member Posts: 4
    Guides need to exactly touch the profiles that are being used and are only done locally.  This loft has two issues:





    Look at this, the start and end profiles look roughly the same.  If they are intended to be the same, I would suggest doing a sweep instead of a loft.  They are far more forgiving for the paths compared to the guides and only need one end profile.  If not, then I would suggest fixing the profile in sketch 16, update the guide in sketch 18 and add guides for the top two points.  On thing that may help going forward is to use the sketch split command where these sketch curves meet to give a vertex to attach a guide to (and create sketch planes on).
    @jakeramsly ;

    Thank you for the feedback Jake! This makes a lot of sense. I didn't know that the points and guides needed to be constrained so precisely. I'm going to give this another shot. As for the sweep option, what are you referring to about using the sketch split for the sweep? I tried do a sweep originally but ran into the same issues of not being able to get it to work. That's actually why I switched to Loft.

    Thanks again!
  • jakeramsleyjakeramsley Member, Moderator, Onshape Employees, Developers Posts: 584
    Guides need to exactly touch the profiles that are being used and are only done locally.  This loft has two issues:





    Look at this, the start and end profiles look roughly the same.  If they are intended to be the same, I would suggest doing a sweep instead of a loft.  They are far more forgiving for the paths compared to the guides and only need one end profile.  If not, then I would suggest fixing the profile in sketch 16, update the guide in sketch 18 and add guides for the top two points.  On thing that may help going forward is to use the sketch split command where these sketch curves meet to give a vertex to attach a guide to (and create sketch planes on).
    @jakeramsly ;

    Thank you for the feedback Jake! This makes a lot of sense. I didn't know that the points and guides needed to be constrained so precisely. I'm going to give this another shot. As for the sweep option, what are you referring to about using the sketch split for the sweep? I tried do a sweep originally but ran into the same issues of not being able to get it to work. That's actually why I switched to Loft.

    Thanks again!
    Hi shane_evans075,

    The sketch split was in reference to the profiles for the loft, not for the sweep.  For the sweep you just pick the path and sweep along it (works best if the path is on the start of the profile).  With loft, splitting the profiles so that they have an explicit vertices is a good way to make the loft more predictable.  Loft tries to line up vertices and maps them across the profiles to figure out which vertex should go with what.  When there is a varying amount of vertices, the loft has to guess where the vertices should be which causes twisting which can cause the loft to try to create something that can't be made.

    An example would be a square lofting to a triangle.  These two profiles have a different amount of vertices, so without any guidance one of the vertices is going to decide by itself where to connect to on the triangle.  The result is a twist in the loft.


    Essentially what I want is for the two vertices that are projected to line up correctly and the other two to be as close to the corners of the square as possible.  I'll draw a construction line to get the point that I want.


    However when I do this and loft, the loft ignore these.  The problem is these aren't vertices of the profile.


    If I edit my sketch again and split at these points, my triangular profile now has 5 vertices.


    Hovering over the line now shows it is two distinct lines.


    As this now gives me 5 vertices and I only have 4 on my square, I am going to split one of the lines of the square.  At this point, I get the loft I am expecting.




    On your sketches, you just have lines that cross one another to create the profile.  There is no explicit vertex at these points.  Without guides at those vertices, it is leaving it up to the system to determine what are vertices and how they should map to one another.  By splitting those intersections you get explicit vertices and can have more explicit control over how the loft looks.
    2.png 51.6K
    3.png 103.4K
    4.png 55.1K
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    7.png 82.5K
    Jake Ramsley

    Director of Quality Engineering              onshape.com
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