Sketching on a face without external references

CURDES
CURDES Member Posts: 4 PRO
edited July 2017 in Community Support
Is there a way to sketch on a face without automatically creating references to the face geometry?

If I have a simple cylinder with a hole and I want to sketch on the end face, can I prevent that hole from becoming part of that sketch? It won't show up as lines but when I go to extrude the geometry, the hole is always included. I'd like to manually add projected curves if I need to reference those edges.

My only workaround is to create a plane each time I want to sketch on a face with a lot of holes/features. Anyone else notice this?

Best Answer

Answers

  • philip_thomas
    philip_thomas Member, Moderator, Onshape Employees, Developers Posts: 1,381 image
    'Imprinting' (copying the face edges to the sketch) should not get in your way. What behaviour is inconveniencing you?
    (and yes, making a plane on the face first is the workaround)
    Philip Thomas - Onshape
  • CURDES
    CURDES Member Posts: 4 PRO
    edited July 2017
    It's a bit of a pain when I want to use a face with a lot of features (holes, pockets) to create a sketch. If I then extrude from that sketch I find myself picking through all of the closed contours to extrude the correct profile. I wish I could make those imprinted edges construction lines...
  • philip_thomas
    philip_thomas Member, Moderator, Onshape Employees, Developers Posts: 1,381 image
    @CURDES - i would like to know more about your work flow.
    Here is a screen capture showing that (in this example at least), that the imprinting has no effect on the subsequent extrusion.

    Perhaps you could make one to show the problem?


    Philip Thomas - Onshape
  • CURDES
    CURDES Member Posts: 4 PRO
    Hi Philip, sorry for the slow reply, I'm not getting notifications from this thread.

    Here is  a link to a public document I've made for an example. If the sketch is intersected by features below it, you must click on separate profiles.

    https://cad.onshape.com/documents/e1b8092957c173a17337d55d/w/dad3e9f8e52d19c112e22861/e/026f528f2902638765c9333e

    In my example I have long shallow pockets as my first feature. I now want to create circular pockets (drawn in sketch 2) on top of those splined pockets . If the spline pocket fully intersects the circle, the profile is split and I must click on the separate parts of the circle. I'd like to have the spline's not imprint so I can just click once on each circle profile.

  • owen_sparks
    owen_sparks Member, Developers Posts: 2,660 PRO
    Yes, this is annoying!

    Even if you hide the part and just have the sketch with the circles visible you can still only select the individual sub regions, inferred from the part below..




    I had this issue with a vac table I'm building, had hundreds of holes that I didn't want to select!

    Owen S.
    Business Systems and Configuration Controller
    HWM-Water Ltd
  • CURDES
    CURDES Member Posts: 4 PRO
    Yes, ok. I'll use offset planes more often

    Thanks!
  • emagdalenaC2i
    emagdalenaC2i Member, Developers, Channel partner Posts: 867 ✭✭✭✭✭
    edited August 2017
    1- You can select the sketch and then extrude
    2- Or you can selec all the faces with a rectangular capture...
    And even better
    3- You can roll back and create first the cut holes and then the spline ones 
    Un saludo,

    Eduardo Magdalena                         C2i Change 2 improve                         ☑ ¿Por qué no organizamos una reunión online?  
                                                                         Partner de PTC - Onshape                                     Averigua a quién conocemos en común
  • owen_sparks
    owen_sparks Member, Developers Posts: 2,660 PRO
    Hi folks.

    Personally I still fundamentally disagree with this behavior.  If I have a single sketch visible and everything else hidden then I don't want these sketch regions to be chopped up into tiny pieces by geometry that I'm not interested in.   I simply want to be able to select regions as defined in the sketch I'm clicking within.

    PT's tip to add an additional plane with zero offset from the face we want the sketch on achieves that, but it's a clever workaround, not a solution. 

    Owen S.
    Business Systems and Configuration Controller
    HWM-Water Ltd
  • konstantin_shiriazdanov
    konstantin_shiriazdanov Member Posts: 1,221 ✭✭✭✭✭
    maybe need to be added one more checkbox in sketch dialog to treat only current sketch regions
  • EvanReese
    EvanReese Member, Mentor Posts: 3,086 PRO
    I wanted to chime in here that I run into issues like this semi-frequently, even though I fully understand how the behavior works. Sometimes the sketch regions are super handy and reduce my clicks, but I think they can get in my way about as often as not. I'd love some way to tell Onshape when I care to use them and when I don't. The Onshape team are the UI masters, so I don't have any real suggestions, but just by way of making sure you know what I mean you might: (1) add a boolean toggle to the sketch itself to recognize them or not, maybe even by auto-creating a plane on the face, (2) Add some way to quickly select regions bounded by sketch geo, not face geo just by where you click (same way that you can select a face or whole surface body by mouse placement). I'm sure an Onshape original solution would be better than either of these, but hopefully, you get the idea.
    Evan Reese
    The Onsherpa | Reach peak Onshape productivity
    www.theonsherpa.com
  • owen_sparks
    owen_sparks Member, Developers Posts: 2,660 PRO
    Oooh, oooh, oooh.

    Have the devs been busy on this, but in super secret squirrel mode?  I've just been using a model and if I hide a sketch then my extrude just picks up on the whole underlying face... Make the sketch visible, then the individual regions are offered as valid selection.  Woo-hooo!!

    Owen S.
    Business Systems and Configuration Controller
    HWM-Water Ltd
  • NeilCooke
    NeilCooke Moderator, Onshape Employees Posts: 6,116 image
    @owen_sparks isn't that just when the sketch is visible you can't select the face underneath it? 

    Senior Director, Technical Services, EMEA
  • owen_sparks
    owen_sparks Member, Developers Posts: 2,660 PRO
    Hi Neil.

    I'm not sure, I've got confused on what the normal behavior was so have gone back to basics...

    Two sketches, each on the top plane.
    Single extrude, of a solid of the sketch regions (not the whole sketch) = 2  overlapping parts.

    I thought they'd fuse into one part, even though the regions are on different sketches.




    Either stuff has changed or I'm just not remembering what normal is.  It's been a long day so I's suspecting the later.

    Cheers,

    Owen S.





    Business Systems and Configuration Controller
    HWM-Water Ltd

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