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Sketch analysis

MatthewMatthew OS Professional, Developers Posts: 22 PRO
is there functionality for checking the validity of a sketch?  In the other systems I've used they either allow you to analyze a sketch prior to using it to create 3D geometry or provide feedback when the sketch is not complete. I've looked for this in the system but have not found it so far. Any help would be appreciated. 

Best Answer

  • andrew_troupandrew_troup Posts: 1,584 ✭✭✭✭
    Accepted Answer
    There is currently feedback as to whether a sketch is closed: when you connect the last entity, the enclosed area becomes shaded.
    Otherwise, there is an indication when you try to create a particular feature type from a deficient or unsuitable sketch. The resulting edit dialog will have a red title, and hovering over that title brings up a description of why the feature failed.

Answers

  • andrew_troupandrew_troup Member, Mentor Posts: 1,584 ✭✭✭✭
    Accepted Answer
    There is currently feedback as to whether a sketch is closed: when you connect the last entity, the enclosed area becomes shaded.
    Otherwise, there is an indication when you try to create a particular feature type from a deficient or unsuitable sketch. The resulting edit dialog will have a red title, and hovering over that title brings up a description of why the feature failed.
  • Narayan_KNarayan_K Member Posts: 379 ✭✭✭
    @ Matthew , By seeing the color of sketch entities we can identify whether sketch is constrained or not.Blue color indicates unconstrained sketch and black color indicates the constrained sketch.
    and we can check the closed and open sketch as  @ andrew_troup explained.
  • brucebartlettbrucebartlett Member, OS Professional, Mentor Posts: 1,879 PRO
    One Improvement which maybe nice is too see where a profile is open, this maybe useful when importing geometry in the form of dxf or dwg with small gaps. Currently I use the method as mentioned by @andrew_troup  to determine if a profile is closed, when I find a profile with an error (not shown to be closed) I will then use a process of elimination by drawing a line across 2 nodes on the profile and checking each side to find the errors.  
    Engineer ı Product Designer ı Onshape Consulting Partner
    Twitter: @onshapetricks  & @babart1977   
  • emmett_weeksemmett_weeks Onshape Employees Posts: 26
    @brucebartlett, another workaround for checking to see if a profile is connected is to use the offset tool and do a drag on it. Offset requires sketch curves to be geometrically connected to form an offset chain. One flaw for this workaround is that it requires two gaps in a loop to find either. I usually use Andrew's approach for small profiles and the offset approach for large ones.
  • andrew_troupandrew_troup Member, Mentor Posts: 1,584 ✭✭✭✭
    @brucebartlett, another workaround for checking to see if a profile is connected is to use the offset tool and do a drag on it. Offset requires sketch curves to be geometrically connected to form an offset chain. One flaw for this workaround is that it requires two gaps in a loop to find either. I usually use Andrew's approach for small profiles and the offset approach for large ones.
    Intriguing (the Offset workaround). Can you explain in a bit more detail what happens with one gap, vs two?
  • emmett_weeksemmett_weeks Onshape Employees Posts: 26
    edited December 2015
    The offset chain will stop on a gap. In the case of a closed loop with one small gap, the gap will be in the offset as well, but you won't be able to see it. If you have two gaps, the offset chain will stop at each and everything between those two gaps will be missing from the offset command. Attached is a polygon that I offset by dragging on one of the lines. There are two gaps in the polygon, one at each end point of the upper left line. If there was only a single gap, the offset would have continued around to every line anyway.
  • andrew_troupandrew_troup Member, Mentor Posts: 1,584 ✭✭✭✭
    edited December 2015
    @emmett_weeks ;

    Very helpful, thanks. I thought that was what you probably meant, but your explanation and illustration is better than mine would have been.  :)

    I use "chain select" in the same way, in Solidworks, because it stops at any gaps, but if there's only one, (as you point out) it travels both ways to get to it and masks it.
    Sometimes I create a temporary break in an easily repaired entity elsewhere, in such cases, to promote it to a 2-gap case..

    The easiest way (on the face of it) would be to delete a straight line and later recreate it between the endpoints of adjacent entities, but there's obviously the risk that the line chosen has the single gap at one end.

    This situation is not only confusing (no promotion to a 2-gap case), but line deletion may lose information (the repaired line may not overlie the original).

    So I generally make my temp gap by sketching a circle *within* an entity, then trim away the segment within the circle, then the circle itself.

    ON EDIT: in the case of gaps where the entities either side are at a pronounced angle to each other, it seems to me emmett's method (vs "chain select") has the advantage of widening the apparent gap, if the offset is to the outside of the bend. If not, it's just a matter of moving the cursor so the offset is to the side which exaggerates the gap.
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