Welcome to the Onshape forum! Ask questions and join in the discussions about everything Onshape.

First time visiting? Here are some places to start:
  1. Looking for a certain topic? Check out the categories filter or use Search (upper right).
  2. Need support? Ask a question to our Community Support category.
  3. Please submit support tickets for bugs but you can request improvements in the Product Feedback category.
  4. Be respectful, on topic and if you see a problem, Flag it.

If you would like to contact our Community Manager personally, feel free to send a private message or an email.

Weird sweep behavior with spline

henry_feldmanhenry_feldman Member Posts: 126 EDU
edited July 2016 in Community Support
Can someone explain what is happening with the sweep along this spline? I was expecting it to be like a loft between the 2 faces, in fact if I select the second rectangle it weirdly goes and does a mirrored sweep, so I am just sweeping one profile. The issue seems to be that the spline isn't normal to the horizontal plane, but it sure seems to be in the sketch (sketch one) although I can't figure out how to make that a hard constraint although since the control handle is set to the same distance from the origin as the end point isn't that perpendicular anyway? (Is there a way to constrain a spline control handle to perpendicular?)

https://cad.onshape.com/documents/9d0289d7fb06d459e29effa6/w/06dbc581e2ab712abdbe6362/e/d3a1953f16a189ee57882ee6

Best Answer

Answers

  • øyvind_kaurstadøyvind_kaurstad Member Posts: 234 ✭✭✭
    I might misunderstand something here, but what were you expecting to happen? If you want the end of the sweep to be in the plane of sketch 3 (top plane in this case), you can use replace face on the end of the sweep and replace it with either the face of sketch 3 or the top plane (will give the same result).

    Perhaps you are being confused by the fact that sweep maintains the angle between the swept profile and the sweep curve/spline? Your sweep profile is not starting off normal to the sweep curve, so it stays off normal throughout the sweep, and therefore ends up like it does.


  • øyvind_kaurstadøyvind_kaurstad Member Posts: 234 ✭✭✭
    Just wanted to add that we really need more and better sweep options. Sweeping along a 3D curve/path is hopeless, since the result will twist in uncontrollable ways. The only shape that can be swept along such a path is a circle, any other shape will result in less desirable results. So please, Onshape, give us better sweep options!
  • henry_feldmanhenry_feldman Member Posts: 126 EDU
    I might misunderstand something here, but what were you expecting to happen? If you want the end of the sweep to be in the plane of sketch 3 (top plane in this case), you can use replace face on the end of the sweep and replace it with either the face of sketch 3 or the top plane (will give the same result).

    Perhaps you are being confused by the fact that sweep maintains the angle between the swept profile and the sweep curve/spline? Your sweep profile is not starting off normal to the sweep curve, so it stays off normal throughout the sweep, and therefore ends up like it does.


    So instead of using one of the primary planes, should I have made a point normal plane to the end of the spline?
  • henry_feldmanhenry_feldman Member Posts: 126 EDU
    Probably. If the sweep profile is normal to the end of the spline, then it will stay normal throughout the sweep. If you want the end of the sweep to be at an angle to the spline (i.e not normal), then you need to use the replace face command for that. That is also currently how you could "stop" the sweep somewhere mid-spline (you would then have some plane/face that the spline passes through, and then after the sweep (which will be along the entire spline), you'd use replace face on the end face of the spline and replace it with the plane/face where you want it to end.


    Thanks. I normalized the face to the spline and that fixed it. The annoying thing seems to be that you can only do that via the spline (It won't let you create a point normal plane to the end point of a spline? Unless there is something I am missing), so I just computed the constraints of the curve handle to be perpendicular to the face...
  • øyvind_kaurstadøyvind_kaurstad Member Posts: 234 ✭✭✭
    You can create a curve point plane at the end of a spline. This plane will be normal to the end of the spline. Just select the spline itself and the endpoint before creating the plane. A curve point plane will then be preselected for you.

Sign In or Register to comment.