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Make a plane by another plane and a line?

I may be missing something obvious, but how to make a plane which is perpendicular to a line on another plane?


Best Answer


  • andrew_troupandrew_troup Member, Mentor Posts: 1,584 ✭✭✭✭✭
    edited November 2015
    I've wondered the exact same thing myself, @alexander_potochkin

    It's trivially easy in Solidworks, but I must admit I haven't nailed it in Onshape.

    I put in an improvement request a while back to modify the way "Line Angle Plane" works to remedy this, suggesting that the default "other" plane be the plane on which the line was sketched, unless the user chose to preselect another plane...

    but the remedy recently implemented by Onshape adopted only the second suggestion, and only indirectly, because it requires specifying a point on the other plane, not just picking the plane (at least, according to the "New in Onshape" demo)  In many cases there will be no point (or vertex) on that plane.

    I look forward to seeing what answers people come up with. It's probably perfectly simple and obvious!
  • peter_hallpeter_hall Member Posts: 196 ✭✭✭
    I too have difficulties with planes. OK if I specify three points, but I could really do with a good video showing how to use/create the various planes using the different methods on Onshape.
  • 3dcad3dcad Member, OS Professional, Mentor Posts: 2,469 PRO
    How about creating a tech tip: How to create planes in Onshape? This would be very welcome for me too.. 
  • ilya_baranilya_baran Onshape Employees, Developers, HDM Posts: 1,156
    For the Line-Angle plane, you can pick a line and any of a number of things, including a point, a plane, and anything that can be interpreted as an axis.  So picking a plane and specifying 90 degrees is the easiest way I think.
    Ilya Baran \ VP, Architecture and FeatureScript \ Onshape Inc
  • andrew_troupandrew_troup Member, Mentor Posts: 1,584 ✭✭✭✭✭
    Thanks @ilya_baran
    I had hoped that would be the case, but hadn't got around to checking it on the off-chance...
    (BTW: Is there a reason the sketch plane could not be the default, in the absence of a user preselection? I imagine there probably is)

    I do wish there was a second-tier, more penetrating summary of new functionality: the one we currently get is pretty much an executive summary at times, and few users will have disposable time to discover the remainder by blue sky research. 

    I realise you have to prioritise the time balance differently than we users do, but in most cases what I'm requesting could just be a bare (textual) list of hints: if we know where to look, we can flesh it out by trial and error. 
  • billy2billy2 Member, OS Professional, Mentor, Developers, User Group Leader Posts: 1,984 PRO
    planes are the x-y axis of a coordinate system. coordinate systems are triple products. 1st direction crossed with 2nd direction, 3rd crossed with 1st creates a coordinate system. This is a geometric standard used by all and transcends all CAD systems. All plane definitions come in this form and may be difficult to understand.

    Try this instead, extrude a sketch as a surface. Then draw on the surface. Perfectly acceptable.

    Create a sketch:

    Extrude as surface:

    cylinders on planes:

    This is a simplified method for generating sketch planes that's more easily understood. Try it and tell me if it's easier to understand.

    This is just a variant on standard geometry creation, a boss on an extruded body. Data wise, it's the same thing.

  • andrew_troupandrew_troup Member, Mentor Posts: 1,584 ✭✭✭✭✭
    One thing I like about planes is that they can be set up, named and searchable in the tree (eg "Forrard starboard galley bulkhead"), globally hidden, remain shown when sketches are globally hidden, and other advantages I can't right now recollect.

    I don't think the problem you're kindly helping to solve, @billy , is intrinsic to planes:
    Solidworks went from being rather problematic to being very good, in terms of plane specification, simply by attending to the creating and editing interface (and, at one point, throwing it out and starting over again)

    Your suggestions will have advantages in some situations, undoubtedly, and it's great to have a variety of options at hand.

    For instance, it strikes me that the ability to create multiple planes in one hit (provided they're all normal to an existing plane or surface) is a great suggestion, particularly given that they need not be contiguous (as your example nicely demonstrates)

    And for individual oblique planes, maybe a transform/rotate about the sketch line? That could be a lot easier to understand, being produced stepwise, than other compound angle methodologies.I've done similar with planes, but the model ends up littered with intermediates, which this alternative procedure neatly vacuums up.

    I think there's probably a lot more depth and applicability in your post than I first realised.

    Thanks, bud!
  • shashank_aaryashashank_aarya Member Posts: 265 ✭✭✭
    edited November 2015
    For plane creation I would like to suggest one enhancement which could be intelligent selection of option after selecting  entities during plane creation. For example suppose I decide to create plane passing through three points, initially it should not be necessarily required to chose the three point plane option but when I pick three points in active plane feature it should automatically navigate to three point plane option. I hope it would be very useful.
    It is already available. Sorry for the post.
  • shashank_aaryashashank_aarya Member Posts: 265 ✭✭✭
    edited November 2015
    Well, @shashank_aarya
    Your wishes have already been answered. Check out the latest 
    Improvements to Onshape - October 29, 2015
    Item 2
    Thanks for sharing the information and sorry for the post. I didn't notice the proper sequence of selection in the video. I was selecting the plane feature first and then selecting the entities but as per current workflow it should be reverse.
  • peter_hallpeter_hall Member Posts: 196 ✭✭✭
    edited November 2015
    @andrew_troup @shashank_aarya     This video helps on getting the plane right , however I would still like an Onshape video showing when each choice of plane type is used and the resulting plane. So far I have worked out midplane, three point, lineangle and offset. Leaves me with Plane point, Curve point and point normal to work out ...........any help appreciated guys. :s
  • andrew_troupandrew_troup Member, Mentor Posts: 1,584 ✭✭✭✭✭
    edited November 2015
    Curve point is a crucial one, because it gives you a plane which is normal (perpendicular) to a selected point (often an endpoint) on any 3D curve, such as the edge between two curvy faces.

    Such a plane is essential for the profile sketch needed to use the edge as the path for a sweep, among other things.

    When we get 3D sketches it will serve a similar purpose for them.

    It could also be used to set up the planes at points along a snake's spine for ribs, or for loft sections to model the snake's body (conceptual abstraction)

    Point normal is (on the face of it) a more limited version of the above, for straight lines only. A straight line can be thought of as a curved line with zero curvature, so it seems the same command could serve for both. However, according to Help, you can optionally define that straight line by (say) selecting a cylindrical or conical or other revolved face or surface (the line being the implied axis of that face) or even just a complete or part circle (implied axis, again), and I can well understand it would get a bit complicated to embrace that rather arcane (and, I have to say, impressively powerful) capability under "Curve Point"

    Plane point (I would personally think of it as "Plane thru point" provides a plane parallel to the given plane passing through the given point.

    It might be useful to think of it like this, though, if you're used to MCAD already :

    It's effectively the end face of a (large) sketch extruded as a solid from the given plane, if you had chosen the given point as the end condition for an "up to vertex" extrusion.

    So it is useful in the interim, to work around the current lack (in Onshape) of that particular end condition. You could define a plane in that way, before performing an extrude.

    - - - - - - -

    Plane definition by the user, I would have to confess, is not currently one of Onshape's crowning glories.

    And the worst case, it seems to me, is "line angle".

    The latest enhancement seems to me something of a bandaid on a wound that ideally needs the attentions of skilled surgeons.

    The fact that they're such a deeply embedded legacy item, being fundamental to the underlying structure of some models, could make it a bit hard to dig them out of what looks to me like a bit of a hole. #

    But legacy holes get deeper at an exponential rate.
    Given we're still in beta, if it has to be done sometime, the present seems to me to be an ideal time to start
    (or it would be more fair to say, speed up) digging.

    Which is my reason (or if it backfires, my excuse) for being outspoken on this matter.

    # On the bright side, they've been so hard to use that perhaps not many existing models rely heavily on them.
  • peter_hallpeter_hall Member Posts: 196 ✭✭✭
    Thanks, had a little play about and managed to set planes using all three commands. Curve point and plane point both worked well and as you said useful on sweeping shapes along a sketch line. Point normal worked in it gave me a plane but appeared to be the same as plane point.....perhaps I wasnt using it with a cylinrical shape on an angled plane. Still it gives me a better insight into creating new planes!
  • clayton_ertleyclayton_ertley Member Posts: 58 ✭✭
    @billy I do the exact same thing.

  • alexander_potochkinalexander_potochkin Member Posts: 44 ✭✭
    Hello everyone

    Thanks again to this wonderful forum I found the right solution to create a plane which is perpendicular to the given line on another plane. Preselecting the plane and the plane + hitting the plane button + setting 90 degrees line angle option
    does the trick.

    Looks like the recent updates do well.

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