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I need help lofting with guidelines

adam_pizzaiaadam_pizzaia Member Posts: 1
edited July 2016 in Community Support
Hello I am trying to loft together the faces on sketch 1 and 2. I want to use the guide lines on sketch 3 to loft them. Onshape will not loft it and I do not know why. Can anyone help?

Answers

  • robert_morrisrobert_morris OS Professional, Developers Posts: 160 PRO
    Lofts can be a tricky thing to get right sometimes.

    Here's a couple of ideas to try:
    1. Separate your guide curves into 2 different sketches and select the actual sketch not the individual curves when specifying the guides.
    2. Try also selecting "Match vertices" and selecting a vertex on each face sketch.
    3. Try re-ordering the face selection (Sketch1 first instead of Sketch 2). That's a weird one, but I've found it sometimes makes a difference.

    I would try #1 first, but it could be a combination of them that ultimately works.

    Hope that helps.
  • Graham_MidgleyGraham_Midgley Member Posts: 1
    Try the Pierce Command at the ends of each line, it is difficult to draw inter connecting lines in different sketches, if the lines don't connect correctly the loft will not work, maybe post a link to your document so we can have a look.
  • chris_8chris_8 OS Professional Posts: 102 PRO
    edited April 2016
    If you mouseover the red "Loft 1" text seen in your image, OnShape will give a general description of the problem. 

    If it says the guidelines must intersect the profiles, then some manual work needs to be done on all four sketches, manually telling those points of intersection to be coincident with both sketches.  Even though they seem to be coincident and maybe they already are, I usually need to manually create those additional constraints, or add a new point and make that be coincident with both sketches.

    If the error message says something about how a body that intersects itself would be created, then maybe more guides will need to be created.  This may be the problem at that bottom 90 degree bend area

  • chris_8chris_8 OS Professional Posts: 102 PRO
    Here's what I would do to make sure the guide lines were intersecting the profiles in a way that OnShape will recognize:


  • chris_8chris_8 OS Professional Posts: 102 PRO
    edited May 2016
    And one more thing I noticed that's causing issues for you:    The guides must each be one entry when creating a loft. In my example each guide was one curve, so each fits into the loft definition as an "Edge of Sketch 3".  However your two guides are 3 segments each, which requires 6 entries.    A way to make one of your line-curve-line combinations into a single entry would be to have each guideline in its own sketch.  So then instead of adding "edge of Sketch 3" you'd be adding "Sketch 3" as one guide, and "Sketch 4" as the other guide.
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