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Cross hatching a rib

vinay_maharajvinay_maharaj Member Posts: 2
edited April 6 in Community Support
Hi experts
I created a rib and sectioned it. As per sectioning rules, I expected the rib NOT to be crossed hatched. Unfortunately, I have a sectioned view with a cross hatched rib. Is there a way to NOT have the rib cross hatched?
Thank you

Answers

  • matthew_stacymatthew_stacy Member Posts: 244 PRO
    @vinay_maharaj, please elaborate.  What are the sectioning rules that you refer to, relating to whether or not ribs should be cross-hatched in a section view?  A screenshot might be helpful as well.


  • NeilCookeNeilCooke Moderator, Onshape Employees Posts: 3,715
    No this is not possible - section rules in standards were primarily included to make a draughtperson’s life easier I imagine. 
    Director, Technical Services, EMEAI
  • PeteYodisPeteYodis Moderator, Onshape Employees Posts: 401
    I've seen older drafting books show this and seen some drawings like this, but I don't know that it's in drafting standards per se.  I do think it actually makes drawings more confusing when you have to know when something appears as not cut - when in reality it is cut by the section.  Are there practical reasons to not show hatching on rib areas, but show hatching everywhere else - even when view generation is doing the work for you?  I suspect the definition of a "rib" can also become very murky at some point.  
  • Henk_de_VlaamHenk_de_Vlaam Member, Developers Posts: 191 ✭✭✭
    @pete_yodis,
    Also in 'old' drafting books but in my opinion still valid: solid shafts should not be cross hatched. This makes a section view more 'understandable and readable'. Is this feature possible in Onshape?
    Henk de Vlaam (NL)
  • PeteYodisPeteYodis Moderator, Onshape Employees Posts: 401
    edited April 6
    @Henk_de_Vlaam Not crosshatched is not necessarily the same thing as not cut.  Not cut is much more common and yes we have plans for excluding from a section, not cutting those parts that are excluded. 

    The request for not hatching a rib, is much more murky and does apply to a piece of geometry within a single part, and in fact it is really cut - but not hatched.  It's cut in examples and if you look closely you see the profile of the rib, but the hatching is not present for it.  @NeilCooke alluded to perhaps on the manual drafting board it did save some time making hatching by hand (and yes, I'm old enough to remember those days).  I suspect it might also be to convey that a part was not uniformly thick in the rib area across the entire part - when it took time to create yet another section view to illustrate that.  Today though, it's pretty easy to make another section view in a different orientation to show the cross section of the rib and surrounding areas.  
  • alnis_smidchensalnis_smidchens Member Posts: 300 EDU
    edited April 7
    For thin features, such as ribs, flanges, etc., the standard/traditional convention is to draw an outline without section lines to clarify that it is a different thickness (or, for some cases, to use different hatching rather than no hatching) while still sectioning the geometry. This is governed by ASME Y14.3 4.2.1 [EDIT: looks like the numbering changes between versions; it may also be filed under 10.3.1].

    However, it is also allowable to use a "true geometry" representation without different hatching (what currently happens in Onshape). I believe SolidWorks allows you to choose whether you want to use a "conventional" or "true geometry" representation when sectioning thin features.

    Here is an example where the thin features are sectioned without hatching:


    Here is one where the section has different hatching:


    Ultimately, I don't think it makes it too much more difficult to understand the drawing if we can't apply different/no hatching to thin features, but I also know some organizations are very particular in the conventions they would like drawings to follow.
    Get in touch: [email protected] | My personal site: https://alnis.dev | My YouTube channel (I make tutorial videos for Onshape & Inventor): https://www.youtube.com/c/AlnisSmidchens
  • Henk_de_VlaamHenk_de_Vlaam Member, Developers Posts: 191 ✭✭✭
    edited April 7
    PeteYodis said:
    [...]  Not cut is much more common and yes we have plans for excluding from a section, not cutting those parts that are excluded. 

    The request for not hatching a rib, is much more murky and does apply to a piece of geometry within a single part, and in fact it is really cut - but not hatched.  It's cut in examples and if you look closely you see the profile of the rib, but the hatching is not present for it.  @NeilCooke alluded to perhaps on the manual drafting board it did save some time making hatching by hand (and yes, I'm old enough to remember those days).  I suspect it might also be to convey that a part was not uniformly thick in the rib area across the entire part - when it took time to create yet another section view to illustrate that.  Today though, it's pretty easy to make another section view in a different orientation to show the cross section of the rib and surrounding areas.  
    @pete_yodis Nice to read that there are plans to exclude parts from cutting.

    And for the rest: The answers from @NeilCooke and you were more or less recognizable to me. In recent years, I have seen it happen in the CAD world that 'a rule' was somewhat dismissed because it was difficult or impossible to implement it in the software at that time. At best a workaround was then suggested. True?  ;)

    Henk de Vlaam (NL)
  • PeteYodisPeteYodis Moderator, Onshape Employees Posts: 401
    @Henk_de_Vlaam Well, we do lots of difficult things - so it's not as much about that.  It's about what things we should or should not be doing.  Sometimes standards do carry over older behaviors and sometimes those are good, and sometimes they are just tradition.  Users and companies sometimes pay attention to standards and sometimes do not.  And those things change a bit over time.  If we are looking to spend our resources wisely it's good for us to have a pulse on how common certain things are.   In my experience the non hatching of ribs was always a bit esoteric and unclear as to why it's helpful - and from my experience in industry not really followed very much and when it is it's more for tradition sake and not necessarily helpful reasons to interpreters of the drawing .  Not many folks in design in manufacturing would reference ASME Y 14.3.  Most will reference ASME Y14.5 which covers dimensions and tolerancing.  At Onshape we certainly want to help our customers create the designs they want and to document them, but it's prudent of us to ask these sorts of questions so that we use our resources most wisely.  


  • S1monS1mon Member Posts: 65 ✭✭
    Does anyone know of a 3D MCAD system which does cross sections without hatching the ribs? I've only ever seen this approach on manually drafted (by hand or dumb 2D CAD) drawings.

    It seems like the reality is that it would be hard to have the system be smart enough to reproduce the hatching the way it's done in the first example @alnis_smidchens posted. The way the ribs join the revolved boss with fillets it would be strange to generate the fake edges where the rib is. If the CAD system has the history of the part, and certain features are marked as "ribs" it could take the section without the ribs and then draw the ribs without hatching. When a system has to deal with imported dumb geometry, this wouldn't be so easy.

    Also, I've worked on so many injection molded parts where you could have philosophical arguments about whether a particular feature is a wall or a rib based on topology and wall thickness. 
  • alnis_smidchensalnis_smidchens Member Posts: 300 EDU
    @PeteYodis I absolutely agree that development time should only be used for features people will actually use! This could be one of those things lots of time and energy is spent on in university which doesn't apply to real-world engineering companies. After all, my structures course this quarter is all about analyzing stresses with a pencil and paper rather than writing scripts to do it with Python or using FEA software!

    @S1mon Here is how you would make this sort of drawing in SolidWorks (there is a pop up after you make a section that asks you to select rib features in the graphics area to exclude from the hatching, so it does require the feature tree):


    What the section view looks like:

    Get in touch: [email protected] | My personal site: https://alnis.dev | My YouTube channel (I make tutorial videos for Onshape & Inventor): https://www.youtube.com/c/AlnisSmidchens
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