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Loft problem.

geoff_joseygeoff_josey Member Posts: 35 ✭✭

I have been trying to progress a fin design for some while without success even after watching the loft related videos etc.
I am trying use the loft function to create a solid between the 2 aerofoil sections which were imported dxf files. One is on the top plane and the second on plane 1
I have a number of error messages. The most common one is that the direction is not known.
Any help appreciated

Best Answer


  • geoff_joseygeoff_josey Member Posts: 35 ✭✭
    Very helpful. many thanks
  • geoff_joseygeoff_josey Member Posts: 35 ✭✭
    I have now run into another problem. I have modified the model to sweep the profile. All looks good and I thought it was solid as that was specified in the loft. When I issue the model for a quote they say the wall thickness is below 0.8 mm ! Not sure why and how do I check that the model is solid ?
  • romeograhamromeograham Member Posts: 534 PRO
    The body is probably solid, but the end of the airfoil is less than 0.8mm:

    Your prototyping supplier may not be able to guarantee that the part that is less than 0.8mm thick will build properly.
    You could cut off the part where it is greater than 0.8mm thick, and resubmit.
  • geoff_joseygeoff_josey Member Posts: 35 ✭✭
    I have asked the supplier to verify the cause of the problem. Awaiting a reply.
    Moving to the next stage. I now want to put a 12 mm dia.hole vertically thro located 144 mm back from the LE at the top. I put the hole on sketch 1 (top face) and planned to extrude it. The introduction of the circle causes an error in the loft. Is my approach wrong ?
  • NeilCookeNeilCooke Moderator, Onshape Employees Posts: 3,539
    Add the hole afterward rather then trying to include it in the loft (loft doesn't like sketches with internal profiles)
    Director, Technical Services, EMEAI
  • geoff_joseygeoff_josey Member Posts: 35 ✭✭
    That is what I tried to do. I have completed the loft and it looks good. I then added a test hole on sketch 1 (top) and tried to extrude with the remove option. I then get extrude and loft errors.
  • NeilCookeNeilCooke Moderator, Onshape Employees Posts: 3,539
    But you edited Sketch 1 which will affect the loft - create a brand new sketch for the hole.
    Director, Technical Services, EMEAI
  • geoff_joseygeoff_josey Member Posts: 35 ✭✭
    Got it - thanks
  • geoff_joseygeoff_josey Member Posts: 35 ✭✭

    With much appreciated assistance from forum members I completed an earlier model involving lofting between 2 aero foil profiles.

    On my current model (see link) I am following a similar procedure ie. importing 2 aero foil sections and then lofting between them.

    The aero foil sections are dxf. files with a fairly high number of points defining the profiles.

    I now get error messages related to the vertices. i have watched the loft video but cannot related my problem to the vertices issues explained.



  • geoff_joseygeoff_josey Member Posts: 35 ✭✭

    I have sorted it ! The problem was extra centre lines on the 2 sketches.

  • romeograhamromeograham Member Posts: 534 PRO

    Also, you may have noticed that you needed to select the face of the sketches, rather than any of the lines that make the edges of the sketch.


  • geoff_joseygeoff_josey Member Posts: 35 ✭✭

    Thanks for you comment. My lofting success rate is still erratic !

    Please clarify your "select faces" comment related to the rudder model.


    I am trying to loft between the 2 outline aerofoils which were imported as dxf files.

    On this example is the face you refer to the plane ?

    I think my problem is in the selection procedure.

  • romeograhamromeograham Member Posts: 534 PRO

    In Onshape, when a sketch has elements that enclose a region (it can be with overlapping lines, or lines that meet at vertices), the region becomes shaded, and selectable.

    Here's your sketch with some lines removed so it doesn't create a closed region:

    Here's the shaded region (showing that the sketch encloses a region:

    For a Solid Loft, Onshape can use the face of the profiles as inputs - so you can just click the shaded region that is enclosed by your sketch elements.

    Another area where you may run into issues when getting started with Onshape is the selection of profiles. If you want to "collect" several selected elements together to be one profile, you can do so, if you use the little drop down arrow in the selection box:

    You can see the 3 edges selected in the first Profile will be connected together as one profile.

    For a surface loft, you need to select edges (of a sketch or body) and for Solid Loft you need to select faces (of sketches or bodies).

    Hope that helps!

  • geoff_joseygeoff_josey Member Posts: 35 ✭✭
    I have tried this loft as a solid and a surface without success,
    I am trying to understand the message " loft did not generate properly Point profiles can only exist as first and last profiles.
    Any help appreciated Thanks
  • romeograhamromeograham Member Posts: 534 PRO
    edited October 2020
    @geoff_josey There are some issues that are making this more difficult than it needs to be. 

    Sketch 1 and Sketch 2 have multiple sets of lines in them. Somehow, the DXFs have duplicate data sets so that when you import them into the Sketch 1, you get two sets of lines "on top" of each other.  This is likely causing you selection issues, so that your features don't complete properly.

    Even though there are extra lines in the sketches, you can still select the face of the sketch and a solid loft completes. 
    With the extra lines in these sketches, I would NOT recommend trying to make a Surface Loft (because a surface loft requires edges as inputs).

    To delete the extra set of lines, you can select each line segment individually, and press the delete key on your keyboard. The sketch will look the same, because there's another line below it (you can't use box-select techniques, because it will select both lines). This will be a lot of work.

    However, you don't need to deal with the lines at all. Some of the lines are creating an enclosed region, which means you can select that to do your loft.

    To make this easier, I used the Offset Surface tool (with 0 offset) to create a surface body (by selecting the face of the sketch). Then you can select that surface face for your loft.

    Create some Guide curves. Use the Bridge Curve to do this.

    Make sure you select points that prevent twisting. I used the points next to the Front Plane:

    Then you can make your selections for a Solid Loft, and use Guide Curves:

    The loft will complete, and won't be twisted.

    There are many, many faces in this loft - and you may have performance issues or difficulty with subsequent features. There are other discussions on the forum about creating a single spline form airfoil data that will likely help. 

    Good luck!
  • geoff_joseygeoff_josey Member Posts: 35 ✭✭
    Many thanks for your help and the great detail. I have been back into the software that created the aerofoil sections and spoken to the originator.
    I was using an obsolete level of the software. When I used the correct level only a single outline was generated. I would have never found this one without your help ! The loft now looks good but I now need to add some more features
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