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Sketching gotchas

thomas_holfordthomas_holford Member Posts: 36 ✭✭
Well, we're making progress here, but we're still fumbling around with sketching problems.

Document: Simpson Strongtie A35 framing angle

https://cad.onshape.com/documents/13e5e699cf0a40cf9565ee0c/w/cb1a6326c0da44a0a1919bb0/e/942f6e556f494b28b82ba6c3

Parts Studio 3

After careful planning with lots of trial and error, I was able to position three imported .DWG drawings representing front, top, and side views on to corresponding OnShape orthogonal planes, Top, Front, and Right.

The edges of the front and top views did not align with the same edges on the side view, so I solved the problem be creating offset planes and copying the drawings to the plans to properly line up the edges.

Question: the newly created planes do not have any labels in the graphics window, whereas the Top, Front, and Right planes are correspondingly labeled.  This is annoying.

As I previously discovered, the imported .DWG drawings needed considerable fixing up to become fully defined. For unknown reasons, some of the drawing lines had end points that were not coincident, at it was necessary to delete some lines and reenter them to create continuous lines.  In the process of re-entering the lines, I entered an erroneous dimension.

OnShape immediately rescaled the entire sketch to be consistent with the new dimension and, in the process, destroyed the alignment of my sketch with the sketches on the other planes.  This was a disaster.

I tried to realign the sketch with the corner of the side view sketch in the another plane using the coincident relationship, but this was unworkable because the sketch was not fully defined.

The imported drawings are, from the point of view of OnSHape, not fully defined because they contain features (hole locations) that are not numerically or geometrically specified in the source drawings.  The hole locations are "free standing" and not dimensionally related to any of the lines, points, or edges of the drawing.

I tried selecting the entire sketch and dragging or transforming it to the correct location, but some of the points or lines in the drawing appear to be fixed and do not drag with other points.

At this point, I think I can see that I can eventually create the part I want to create, but it will require a lot of fix ups, do-overs, and work arounds.

A key problem is the difficulty of manipulating, editing, and positioning sketches.  And also, it seems that OnShape could or should be a lot more helpful with regard to importing .DWG files. Right now, it seems to do the bare minimum to get the .DWG drawings into the OnShape environment.  But whether or not anything useful can be done with them is a problem for the user to figure out.


Answers

  • brucebartlettbrucebartlett Member, OS Professional, Mentor, User Group Leader Posts: 2,119 PRO
    I had a bit of a look at part studio 3. Your right the imported geometry is not real easy to work with as everything comes in unconstrained you then have to work though each line to add the constraints as required. It might be almost easy to start from scratch automatic inferencing.

    A few tips that might help get your sketch fully constrained if you have not already worked them out:
    • Switch the "Show constraints" on in the sketch dialogue.
    • The "Fix" constraint is a good to start with just window select all lines or the major lines and fix. I normally would try and get rid of these after everything else is constrained. 
    • The Trim "Extend" can be used to put constraints on the corners.
    • You can accumulative select or window select vertical or horizontals and knock them over in 1 go.
    • You can window select then RMB to copy sketch entities then RMB paste sketch entities in a new sketch take constraints as well. This could be handy to pull bits out of a imported sketch.
    Hope that help's 


    Engineer ı Product Designer ı Onshape Consulting Partner
    Twitter: @onshapetricks  & @babart1977   
  • andrew_troupandrew_troup Member, Mentor Posts: 1,584 ✭✭✭✭✭
    The Trim command in Onshape could do to be more powerful, I'm starting to think.

    For a start:
    User should be able to click on two entities, to whichever side of their intersection is to be kept, and the lines should mutually trim/extend, and merge.

    The relative lack of focus on trimming made sense to me at first assessment, because in the native Onshape environment, sketches do not NEED to be trimmed ...  but what some of us are starting to realise is that above a certain level of sketch complexity, the cognitive overload makes untrimmed sketches, even native ones, a liability.

    And for badly drafted imported sketches, it's essential to have more tools. Many new users will not have a suitable 2D package, or the desire to step back in time to learn to use it, to check and repair geometry prior to importation, and this workflow would be inefficient even for shellbacks.
  • andrew_troupandrew_troup Member, Mentor Posts: 1,584 ✭✭✭✭✭
    A note to new users: the problem the OP struck was caused by geometry which did not meet, but where the gap was too small to see. 
    There's no problem in Onshape with untrimmed entities which overlap the intersection.

    The problem the OP had with inability to move the sketch could probably have been resolved by using "Derive", and moving the derived sketch using "Transform" - this was suggested in another one of his threads - he may care to explain what the problem was with applying that suggestion.

    Another suggestion was to use the imported sketch as an underlay, and create a new sketch offset from it, taking advantage of "Use/Project" to pull geometry from it. This would avoid the need to constrain geometry. (The first sketch could have all elements box-selected, and "Fixed", for maximum security.)

    Again, it would help everyone if the OP would enlighten us as to why this didn't work for him.
  • thomas_holfordthomas_holford Member Posts: 36 ✭✭
    A note to new users: the problem the OP struck was caused by geometry which did not meet, but where the gap was too small to see. 
    There's no problem in Onshape with untrimmed entities which overlap the intersection.

    The problem the OP had with inability to move the sketch could probably have been resolved by using "Derive", and moving the derived sketch using "Transform" - this was suggested in another one of his threads - he may care to explain what the problem was with applying that suggestion.

    Another suggestion was to use the imported sketch as an underlay, and create a new sketch offset from it, taking advantage of "Use/Project" to pull geometry from it. This would avoid the need to constrain geometry. (The first sketch could have all elements box-selected, and "Fixed", for maximum security.)

    Again, it would help everyone if the OP would enlighten us as to why this didn't work for him.
    "Derive" is a very obscure function.  It's not mentioned in any of the video tutorials I viewed, and there is no entry for it in the Help index.

    "Transform" would be wonderful, but my experience is that it does not work on sketches, and that's what the Help entry seems to say:

    "Transform adjusts a part's location and orientation in 3D space with the option to copy the part in place."

    The ability for Transform to operate on sketches would make things a lot easier.
  • thomas_holfordthomas_holford Member Posts: 36 ✭✭
    Just a general comment about this particular project:

    I realize that there are potentially multiple approaches to achieving the end result I'm looking for.  However, for the time being I'm trying to work through an approach where I can import multiple drawings into sketches in one Part Studio to create one part.  I'm doing this to get a better understanding of the capabilities and advantages creating related parts in one operation.

    Earlier, I tried an approach that created the blades of the parts as separate parts in separate Part Studios, and assembling them using mates.  I see no reason why this  wouldn't work, as well.

    I'm also beginning to realize that  combining front, side, and top drawings may be a common requirement for  turning zillions of archived drawings into 3D models.  It would be good to know how to do this quickly and efficiently.
  • andrew_troupandrew_troup Member, Mentor Posts: 1,584 ✭✭✭✭✭
    @thomas_holford
    You make some valid and instructive points.
     
    But first, yet another tip (and I promise this one is not as misleading as your post reveals a couple of my previous tips to have been)

    When searching in help, it pays to ignore the search in the left window. Go to the search box at top right, and you will find "Derived" is covered, starting with the words

    "Insert a geometric feature from one Part Studio into another in the same document...."  

    so my advice to use Derive within the same part studio was unhelpful, and the only workaround which immediately suggests itself (a "round trip" into a dummy studio) not very attractive.

    Second misleading tip: You are exactly right about Transform not working on sketch geometry. (Yet)
    I could plead in mitigation that I was encouraged to believe that by tips from others, and furthermore that the product is evolving so fast it's difficult to keep clear-headed as to what currently works, but neither of those claims constitutes an excuse.

    Sorry to have led you an unfruitful chase.
  • brucebartlettbrucebartlett Member, OS Professional, Mentor, User Group Leader Posts: 2,119 PRO
    I'd stay away from the derived sketch and just copy and paste your views in to new sketches with the  the RMB "copy/patse sketch entities"

    Check out the sketches in this studio, these are constrained well to my way of thinking, very easy to copy out and reuse with constraints in tact:
    https://cad.onshape.com/documents/0a355a367a4941eca0d90a0f/w/3d4fdaaf6b77419db7fa309b
    Engineer ı Product Designer ı Onshape Consulting Partner
    Twitter: @onshapetricks  & @babart1977   
  • andrew_troupandrew_troup Member, Mentor Posts: 1,584 ✭✭✭✭✭
    edited September 2015
    It looks to me as though, while "Derived Parts" may well be ready for thorough beta testing, "Derived Sketches" suffer from so many limitations and deficiencies that they're currently just a tantalising glimpse of the possible.

    Once they work properly (including, but not limited to, the very useful and productivity-enhancing functionality in Solidworks) they will be a real asset to Onshape.
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