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What are the rules for inheritance of elements with subelements

baumarbaumar OS Professional Posts: 38 PRO
I designed an larger part containing e.g. holes. When I extrude the circles were recognised and extruded correctly as holes.
Then I add another sketch on the face of that extrusion. I created a e.g. rectangle including some of the holes and made another extrusion.
In one workspace it created 1 part with the holes taken from the face as expected. In another design it created each hole as a separate part, but I couldn't figure out the rule.
Can anybody explain, how of an underlaying plane the surrounding element and the elements within that element are inherited to the next part?
thanks for help
  

Comments

  • john_mcclaryjohn_mcclary Member, Developers Posts: 439 PRO
    I'm not sure I fully understand your question, but...

    Are you having a problem, are you trying to figure out the solve order of features in OnShape, or are you trying to figure out a design strategy with part studios?
  • NeilCookeNeilCooke Moderator, Onshape Employees Posts: 1,047
    Sketching on a part face and sketching on a plane will give you different results. A part face will give you extra regions to select and therefore if there are multiple loops you may get different results than what you were expecting. When extruding from a part face you will probably need to select the regions rather than the whole sketch. 
    Neil Cooke, Director of Technical Marketing, Onshape Inc.
  • baumarbaumar OS Professional Posts: 38 PRO
    Thanks Neil for the hints, however the behaviour is not yet clear to me. And sorry John, I agree my question is a bit too abstract. 
    What was not clear was your words: "you will probably need to select the regions rather than the whole sketch"
    The question is how to select. I noticed that the result was different when clicking on an element (e.g. the rectangle containing other elements inside) or by selecting it with the mouse, when you drag another rectangle around the rectangle containing the other elements. 
    Since you wrote probably, I seemed to me you're not sure about the effect either, so I made an example to visualise the effect.

    https://cad.onshape.com/documents/21210f6571649c65da2bb65e/w/f80b48c99ff05d3c9ed9a252/e/2037c32f71f691dbafb4726b#
    with comments on the extrusions how this was done. 

    It seems to me that the behaviour is even more complex then described by Neil.

    In this example I checked the behaviour in the following scenarios: 

    Scenario 1 all figures with concrete lines in the same sketch 

    Extruding from a sketch with concrete lines, and then extruding from the back (Extrude 1 and 2)
    The special thing was that only in this example I was able to select for both extrusions the sketch. (For all following examples I could only select the face for the second extrusion). 
    As described in the comments Extrusion 1 was done by selecting the surrounding rectangle with the mouse (draging around the whole rectangle), Extrusion 2 by clicking with the mouse

    Scenario 2 Creating a sketch with construction lines, then create another sketch with concretisation of ALL elements (here rectangle plus holes inside of rectangle). 

    Extrusion 3 - 6:


    Extrusion 3 was selected with the mouse by dragging a rectangle  around the rectangle, Extrusion 4 by selecting the face of Ext3, it was not possible to select the plane. The whole were not taken

    Extrusion 5 was done by clicking the rectangle, Ext 6 by selecting the face of Ext 5, again no selection of the sketch was possible. Only here the holes were taken. 


    Scenario 3 concrete figures distributed on 2 sketches (here holes in sketch 1, rectangle in sketch 2)

    Extrusion 7-8

    The result doesn't seem stable. First I had a selection that showed the whole, but then I created a second figure to compare again clicking the rectangle and selecting the rectangle by dragging the selection with the mouse around. 

    To make this quickly, I mirrored as well the figure sketch 1 and sketch 2. 
    When dragging /selecting with mouse, the inner circle was recognised and shows on the surface with that funny blurring surface, but the hole is not made. When clicking the rectangle the hole is not selected at all. 

    Now I don't think this really intuitive and it caused me quite some headaches in designing because if you don't clearly understand the mechanism it is hard to get the right thing. 

    Is there ( or will there be 8-)  any description or video how these selections mechanism work? I think that would be very useful to do it first time right, it took me a lot of time to discover the huge difference of small differences in design (strategy) and I think I still don't understand it correctly. 


  • john_mcclaryjohn_mcclary Member, Developers Posts: 439 PRO
    Ok I think I get it now.

    You are making an extrusion from a sketch, then you try to select the sketch from the 3D area and instead you are selecting the part face of the part "behind" the sketch.

    Right?

    This was a long explanation, so I just made a video instead. I hope it helps

    https://youtu.be/Z0pGq_D84mg
  • rbaekrbaek Moderator, Onshape Employees, Developers Posts: 77
    edited April 12
    Hi @baumar, if I may I will breakdown what is happening for each Extrude in your document.
    • For Extrude 1, you selected the rectangular region and the 3 holes, thus the result is a block. What you did here is select each sketch region (the rectangular region, and each of the three holes). Clicking them individually will have the same effect as box selecting (click and drag) these regions.
    • For Extrude 2, you only selected the rectangular region (which excludes the three holes), thus the result is a block with 3 holes.
    • Extrude 3 is the same as Extrude 1, where you box selected all 4 regions and thus the result is a block.
    • Extrude 4 is where you selected the face of Extrude 3, which is just a flat plane with no sketch regions. If you wanted to extrude the sketch region with the holes removed, you would need to select the sketch, not the extrusion.
    • For Extrude 5, you again select only the rectangular region, thus having the same result as Extrude 2.
    • For Extrude 6, it is the same result and selection as Extrudes 2 and 5.
    • For Extrude 7, you selected both the rectangular region as well as the hole, but with the New Extrude type, thus resulting in two parts. The reason why you cannot achieve a block with a hole, is because the rectangular region belongs to the first sketch, while the hole belongs to the second sketch; thus when you extrude, selecting both regions will create new parts that overlap. If you wish to achieve a block with a hole, both the rectangular region and the hole should either be in the same sketch, OR you can do an extrude remove if those regions are in separate sketches.
    • For Extrude 8, you have a construction circle, so there is no hole created by selecting the rectangular region.

    Some points that may help understand why the behaviors are as such above:
    • Extrusions only work with solid sketch geometry regions
    • Sketch regions in different sketch features will have different effects when extruding compared to having those regions in the same sketch feature.
    • Selecting a sketch region from the graphics area, box selecting the sketch regions, and selecting the sketch feature from the feature list all will have slightly different effects (catering to all types of workflows).
    • Box select and clicking individually have the same effect; they are just different methods of selection.
    This is a result of our multi-part environment of Part Studios which is an experience unique to Onshape. It may be confusing at first, but this is a powerful tool that allows users to create multiple parts in one tab.
    I hope this helps.
  • baumarbaumar OS Professional Posts: 38 PRO
    Hm, I don't know what I should say. First I would like to thank you for your extended answers to my questions.
    Some of the explanations or effects remain ambiguous. Maybe my question was not clear enough inspite of the effort I spent to visualise it with the model. 

    But instead of struggling about some details I would like to come back to my main question: I am searching a clear explanation, maybe with a demo/or video, so I can understand that "multi-part environment behaviour". You say "It may be confusing at first, but this is a powerful tool that allows users to create multiple parts in one tab". 
    It remains confusing, because I didn't get a clear description how it works. 

    In the design I'm working on, there are some holes that have to be propagated through several parts. If in the 4th or 5th layers they are not propagated anymore because I didn't understand the mechanism, this is not only confusing, but frustrating. I have spent hours to find out with experiments, but I this try and error way is a bit cumbersome. 

    So if there were parts in the documentation or in videos describing this mechanism that would be great help. 

    Thanks for your support. 

  • billy2billy2 Member, OS Professional, Mentor, Developers Posts: 827 PRO
    Don't forget you can pick the sketch from the feature tree and avoid all that region stuff.

    Don't get me wrong, I like the region stuff and use it a lot.


  • lanalana Onshape Employees Posts: 192
    @baumar
    You might be implying some cleverness that is not there. Extrude uses exactly the set of faces you select as its input. They might be faces created by sketch (shaded areas in the sketch) or any planar faces. When sketch is created on a face(vs. construction plane) this face boundaries contribute to sketch face creation.

    Construction entities of sketch don't contribute to sketch face creation.

    When selecting input for extrude you can pick faces one-by-one or select sketch feature ( select it from feature list or pick extrude button while in sketch dialog). This creates a slightly different selection, we call it sketch region. It resolves to connected sketch faces within external sketch contours, but outside internal ones. Discussed here in more detail. We advise using this selection whenever suitable because it is most stable towards sketch changes.
    I hope this makes sense.
  • baumarbaumar OS Professional Posts: 38 PRO
    Hei guys, I found the solution just in one of the videos - the use command. I don't think I had this when I was designing this.

    That's the key: you want to use the same geometry in different planes. but so far, I had to redesign it manually, as there was no way to propagate it (or I was not aware 8-). This is bad, because when in the master sketch a change is made, it is not propagated. With the use command this seems to be solved.

    and thanks a lot for the link to https://www.onshape.com/cad-blog/extrude-logic-and-sketch-resilience, that is very useful!

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