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Snapping to Existing Geometry

matthew_65matthew_65 Member Posts: 6
In Sketch Mode, entities I create do not snap to existing edges.  I am a Creo user, used to creating "sketch references" from existing geometry, which effectively projects a construction entity onto the current sketch.  How do I do this in Onshape?

Best Answer

  • jakeramsleyjakeramsley Member, Moderator, Onshape Employees, Developers Posts: 642
    Answer ✓
    Currently, our inferences are to:
    1) The origin as long as the origin is visible.  You can inference horizontal, vertical, and coincident with the origin with no need to wake it up.

    2) Sketch geometry in the same sketch.  If you hover over sketch geometry from the same sketch while a sketch tool is active, this will "wake up" the inference to that geometry allowing you to make constraints like coincident, mid-point, parallel, perpendicular, etc.

    3) Edges of the sketch face.  If you are sketching on a face, you can infer to all of the edges and vertices that make up that face.
    Jake Ramsley

    Director of Quality Engineering & Release Manager              onshape.com

Answers

  • lougallolougallo Member, Moderator, Onshape Employees, Developers Posts: 1,995
    @Matt Coté Currently we disable inferencing on entities that are not on the same plane as the sketch.  We have been working on ways to wake up more common inferences but can you share which situations you are looking to get inferences on?  
    Lou Gallo / PD/UX - Support - Community / Onshape, Inc.
  • matthew_65matthew_65 Member Posts: 6
    In my case, I am simply trying to snap sketch entities to existing geometric edges which lie on my current sketching plane.  In the tutorial videos I have watched, it appears that, as the mouse moves over existing edges (while in sketch mode), snapping inferences automatically appear.  This doesn't happen for me.  Is there a setting somewhere which allows me to turn on "auto snapping" or "auto inferencing"?  I have tried preselecting an existing edge, thinking that Onshape might "remember" that selection while sketching, but that does not work.  I must be missing something obvious, no?
  • jakeramsleyjakeramsley Member, Moderator, Onshape Employees, Developers Posts: 642
    Answer ✓
    Currently, our inferences are to:
    1) The origin as long as the origin is visible.  You can inference horizontal, vertical, and coincident with the origin with no need to wake it up.

    2) Sketch geometry in the same sketch.  If you hover over sketch geometry from the same sketch while a sketch tool is active, this will "wake up" the inference to that geometry allowing you to make constraints like coincident, mid-point, parallel, perpendicular, etc.

    3) Edges of the sketch face.  If you are sketching on a face, you can infer to all of the edges and vertices that make up that face.
    Jake Ramsley

    Director of Quality Engineering & Release Manager              onshape.com
  • matthew_65matthew_65 Member Posts: 6
    Thank you very much.  Very helpful and informative.
  • ShepRCSShepRCS Member Posts: 9
    I can see this being one of those "careful what you wish for" requests where the document is covered in glowing snaps.  but I am also after the ability to snap to entities off the sketch plane.

    Shafts - If I create a shaft and then want to create a revolve a part on that shaft there is not quick way to get the hole in my part the same diameter as the shaft.  I want to be able to snap the edges of cylinders. At the moment I have to use the end of the cylinder and snap some construction lines to the end of the resultant line.

    the current disabling of entities not on sketch plane actually seems to further than that. Its actually entities not on the face you selected to draw the sketch on.  Where you have two adjacent parts and you select one of the adjoining faces as your sketch plane you can't use entities from the other part to snap to. if you could at least turn on all entities on the sketch plane that would be good!  Beyond that a way to wake up relations to other parts would be excellent.  

    Back in my old autocad days I like being able to specify the snaps whilst drawing the object. it meant I could specify mid and be sure that any auto snaps appearing where in fact mid points.  Maybe OnS could have a similar system? Or even better the program could learn what snaps the user habitually uses and present those preferentially!

    Shep
  • jakeramsleyjakeramsley Member, Moderator, Onshape Employees, Developers Posts: 642
    Internally we've gone through a couple of iterations of sketch inferences.  In my opinion, there was nothing more annoying and barrier to my design than having too many inferences.  Every little mouse movement snapped to something and forced me to have to either hold shift to suppress the inferences the entire time or do a ton of clean up after.  There's further configuration to be done with sketching and inferences, but I think there is some leg work to be done in front of that.
    Jake Ramsley

    Director of Quality Engineering & Release Manager              onshape.com
  • 3dcad3dcad Member, OS Professional, Mentor Posts: 2,466 PRO
    @JakeRamsley
    That is so true, I hate it when you can't move freely but all the time snapping into something. I'm a big fan of multi-part design and if sketches would auto-snap into everything in the background - it would be very annoying.

    In my opinion snapping is very good at this point, when creating a geometry auto-snap gives you needed space not picking everything and when tool is disabled it finds all instances in the background - except mid-point +1 for finding these too.

    Often I try to end geometry NOT snapping into anything then zoom in and use constraining tools to be sure what is connected to where (and how).
    //rami
  • 3dcad3dcad Member, OS Professional, Mentor Posts: 2,466 PRO
    I would like to see enhancement in 'Select other' though, I would like to use keyboard shortcut to change selection when hovering. This could be in addition to RMB > Select other so it wouldn't bother anyone not needing it as much as I do. 
    //rami
  • matthew_65matthew_65 Member Posts: 6
    Thanks, everyone.  Man, you guys are prompt!  :-)
  • andrew_troupandrew_troup Member, Mentor Posts: 1,584 ✭✭✭✭

    +1 for some quick way to "drill down" to the desired inference point to snap to.

    Filters on Sldwks were effective, but labour intensive.

  • _Ðave__Ðave_ Member, Developers Posts: 712 ✭✭✭✭
    Matt Coté When I want a inference that is not on the same level/depth as the sketch plane. First I will create the geometry with no inference then I will select that geometry and the feature I want to inference then just select the coincident, concentric or whatever inference I wish. Appears to work or I just didn't understand the issue.
  • paul_breedpaul_breed Member Posts: 16
    I personally like the Rhino interface where I can selectively turn individual snap types on and off, point, end, center, mid, tangent,  That way if I have lots of items close together I can force it to use the only the class of snap I want
  • sam_barkersam_barker Member Posts: 1
    When you have separate entities and select only one face from one entity as your reference plane for the active sketch, other surfaces (though on the same plane) will not activate for "snapping" unless the "Use (Project/Convert) (U)" tool is used. After selecting the reference plane, press "U" and then select the other surfaces that you want active during your sketch. This made all the difference when I finally figured it out. 

  • andrew_troupandrew_troup Member, Mentor Posts: 1,584 ✭✭✭✭
    @sam_barker
    By "surfaces" I imagine you mean "faces"?
    (In solid modelling terminology, the former refers to infinitely thin surfaces, created in isolation from solids; the latter refers to the faces of a solid body.)

    Thanks for sharing this tip; I look forward to getting to grips with how to apply it.
  • joesoupjoesoup Member Posts: 2
    edited June 2016
    I need this too, badly. I can unstained how it could get int the way, but why not have a switch where you can turn it on and off snapping?
  • chris_8chris_8 OS Professional Posts: 101 PRO
    I could use more snapping abilities most every part that I create.   Manually clicking on points and lines, then choosing coincident to set them as coicident seems like unnecessary redundancy.

    The concerns some have stated about everything highlighting and thereby causing problems makes sense in some cases.   So the idea of having the ability to wake or put to sleep such recognition seems like a great solution.
  • gskgsk Member Posts: 5 PRO
    To be honest, I simply cannot understand the explanation that this is not implemented, because it would be a mess, everything will be highlighted etc. SolidWorks has this feature and it works great. In case I need to draw on offset plane "in context" by repeating some (not all) geometry of another part and extruding new feature/part up to part, the lack of snap does decrease usability a lot.

    SolidWorks example:
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