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Another design contest

emagdalenaC2CemagdalenaC2C Member, Developers Posts: 410 ✭✭✭✭
edited May 29 in Using Onshape
The contest as usual is to design this part with the least number of features:


Rules:

- The number of slots may vary

- All slots are tangent to the faces of the cylinder with an offset of A millimeters

The best answers will be marked as accepted answers ;-)

Good luck  ;)
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Best Answers

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Answers

  • emagdalenaC2CemagdalenaC2C Member, Developers Posts: 410 ✭✭✭✭
    Extra points if someone manages to make the drawing correctly dimensioned  >:)

    PD: One of these days we will make Onshape break with this game  o:)
    Un saludo,                                                      C2C Close 2 Circle™                                   ☑ ¿Por qué no organizamos una reunión online? 
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  • john_mcclaryjohn_mcclary Member, Developers Posts: 932 PRO
    I assume custom FS is out?
  • emagdalenaC2CemagdalenaC2C Member, Developers Posts: 410 ✭✭✭✭
    FeatureScript should be out... but:
    1) A macro in FeatureScript would actually use other design operations as a base, so it makes sense to first try to do the design and then automate it with FeatureScript
    2) I would love to see a FeatureScript for this example
    Un saludo,                                                      C2C Close 2 Circle™                                   ☑ ¿Por qué no organizamos una reunión online? 
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  • brucebartlettbrucebartlett Member, OS Professional, Mentor Posts: 1,616 PRO
    edited May 29
    Here's my attempt, 14 features including a variable for the number of slots.

    https://cad.onshape.com/documents/c4ba2cbb65d395eeb3d2009f/w/7d6175fc813e559e009c547e/e/5f281deafc8d6fbf12fc26f6
    Engineer ı Product Designer ı Onshape Consulting Partner
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  • emagdalenaC2CemagdalenaC2C Member, Developers Posts: 410 ✭✭✭✭
    You are close... but there are a few issues ;-)


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  • emagdalenaC2CemagdalenaC2C Member, Developers Posts: 410 ✭✭✭✭
    I am still not perfect on the top dim but that's the best I can do, for now, I had to add an extra measure feature too. It is a bit of a challenge thanks.
    Thank you very much ... Yes, it's not perfect yet but you're getting closer
    Un saludo,                                                      C2C Close 2 Circle™                                   ☑ ¿Por qué no organizamos una reunión online? 
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  • emagdalenaC2CemagdalenaC2C Member, Developers Posts: 410 ✭✭✭✭
    edited May 30

    It's exactly the same as what I got.
    Although I have one less operation... because I did not eliminate the surfaces ;-)
    https://cad.onshape.com/documents/98c43f730cc7deb2d25486e7/w/988e18dbc7c3f809e9da275c/e/9c7eb4a95229a265fa805dbf
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  • larry_haweslarry_hawes Member Posts: 271 PRO
    Great work and very interesting. Could someone explain the circular pattern and why the cutouts are truncated at the bottom of the plane, which I assume is there for that purpose. I see that checking the "Apply per instance" box will cut the cutouts to their proper location but really don't understand that feature.

    Thanks
  • john_mcclaryjohn_mcclary Member, Developers Posts: 932 PRO
    It's because they are wizards Larry!

    It's amazing some of the black magic I've seen people do in onshape.

    I really need to learn how to think abstract like that too.
  • brian_jordanbrian_jordan Member, Developers Posts: 106 ✭✭✭
    Fascinating! Something more learned here, particularly with the way the slots are formed, but is the choice to dimension the thickness to 10 rather than the inner diameter as 80 in sketch 1 for performance, personal choice or some other reason?
  • emagdalenaC2CemagdalenaC2C Member, Developers Posts: 410 ✭✭✭✭
    but is the choice to dimension the thickness to 10 rather than the inner diameter as 80 in sketch 1 for performance, personal choice or some other reason?
    For other reason ... simply for annoying ;-)
    In the sketch it is easy to add that dimension, but in the drawing... well, it is not so simple
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  • mbartlett21mbartlett21 Member Posts: 788 EDU
    Accepted Answer
  • emagdalenaC2CemagdalenaC2C Member, Developers Posts: 410 ✭✭✭✭
    Actually I did the same yesterday ;-) and without delete surfaces, so 7 features
    https://cad.onshape.com/documents/98c43f730cc7deb2d25486e7/w/988e18dbc7c3f809e9da275c/e/b9028454f0634d679840eab5

    But there are still some problems with the accuracy

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  • larry_haweslarry_hawes Member Posts: 271 PRO
    It's because they are wizards Larry!

    It's amazing some of the black magic I've seen people do in onshape.
    Too true, too true. It also seems that some of that black magic is exactly that and hidden within the interface from the every day user but I learn something new with each one of theses 'contests'.
  • NeilCookeNeilCooke Moderator, Onshape Employees Posts: 1,519

    But there are still some problems with the accuracy

    My first incarnation was without plane but accuracy was worse. I can only assume that it is something to do with the surface boundary (even though the surface definition is flat). I also tidied the surfaces up from habit. 

    I see that checking the "Apply per instance" box will cut the cutouts to their proper location but really don't understand that feature.

    Thanks

    “Apply per instance” recalculates each feature of the pattern and is required to change the length of each extrude. 
    Neil Cooke, Director of Technical Marketing, Onshape Inc.
  • emagdalenaC2CemagdalenaC2C Member, Developers Posts: 410 ✭✭✭✭
    I have tried several options to improve the accuracy but I have not improved the result.

    https://cad.onshape.com/documents/98c43f730cc7deb2d25486e7/w/988e18dbc7c3f809e9da275c/e/64b98f6e37be229b12e4dd2d

    As you can see in the document, it is relatively easy to obtain a variable linear pattern (See Part Studio Matriz lineal variable)



    But in this example, the most accurate result I get is the one you can see in Part Studio 5 (with 15 features, and without the option to automatically change the number of slots)
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  • larry_haweslarry_hawes Member Posts: 271 PRO
    NeilCooke said:

    “Apply per instance” recalculates each feature of the pattern and is required to change the length of each extrude. 
    Yes, I found some references to same on the web but could find no indication of why the length of each extrude was changed to (apparently) match the plane's location, if indeed that was even the case? It simply looks like magic from here and I think you and your fellow magicians are hesitant to share your magic tricks' secrets :) :smiley:
  • lanalana Onshape Employees Posts: 313
    @larry_hawes
    This is actually a perfect opportunity to discuss "Apply per instance" option in more detail because this is a rare use case when its use is necessary. When patterning extrude with up-to-face bounding condition with "Apply per instance" option, for each instance a copy of the profile to be extruded is moved according to pattern transformation and then extrude of that copy is created. In each location the extrude reaches to the bounding face.
  • john_mcclaryjohn_mcclary Member, Developers Posts: 932 PRO
    Will there ever be a true "advanced modeling" webinar?  That showcases some of these kinds of examples?
  • larry_haweslarry_hawes Member Posts: 271 PRO
    lana said:
    @larry_hawes
    This is actually a perfect opportunity to discuss "Apply per instance" option in more detail because this is a rare use case when its use is necessary. When patterning extrude with up-to-face bounding condition with "Apply per instance" option, for each instance a copy of the profile to be extruded is moved according to pattern transformation and then extrude of that copy is created. In each location the extrude reaches to the bounding face.
    Yes, but where is the 'bounding face' selected or noted in this design contest model? Is it the plane? How does Apply per instance locating that plane, if it is, in this model? Circular pattern doesn't seem to have that plane or any other 'bounding face' selected or noted? Or if it does it is certainly not clear to this (not so bright sometimes) user.
  • brucebartlettbrucebartlett Member, OS Professional, Mentor Posts: 1,616 PRO
    Hi @lana,  I have this version I was trying to get the work by using a sketch that was referencing the top face which I was expecting to update via per instance. When I started this version it seemed like some of the instances to were changing but then I as I kept modifying it stop working. Should this work or not? https://cad.onshape.com/documents/c4ba2cbb65d395eeb3d2009f/w/e7c87743cb563ced4c73b0e5/e/5f281deafc8d6fbf12fc26f6
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  • lanalana Onshape Employees Posts: 313
    edited May 30
    @larry_hawes
    Using @emagdalenaC2C ; document as an example: Bounding face is in the definition of Extrude 3:  


    @brucebartlett

    You've caught an internal shortcut :) - within feature pattern "Apply per instance" option sketches are resolved ignoring constraints to out-of-sketch geometry. This is a good example for where such constraints could be useful. Unfortunately too often they cause unexpected results.
  • larry_haweslarry_hawes Member Posts: 271 PRO
    edited May 30
    lana said:
    @larry_hawes
    Using @emagdalenaC2C ; document as an example: Bounding face is in the definition of Extrude 3:  



    I don't doubt that you are correct but would anyone but an (uber) expert understand that from the model? And why doesn't the circular pattern dialog box refer to it? Or does it? If so how? If not why not?
  • emagdalenaC2CemagdalenaC2C Member, Developers Posts: 410 ✭✭✭✭
    @jon_sorrells there are some interesting features in your model, but:
    - The slots are not normal to the cylinder
    - The distance of the slots to the sloping face, as in other models, is not correct
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  • emagdalenaC2CemagdalenaC2C Member, Developers Posts: 410 ✭✭✭✭
    Accepted Answer
    For those who want a more detailed explanation of my model (Part Studio 4):
    https://cad.onshape.com/documents/98c43f730cc7deb2d25486e7/w/988e18dbc7c3f809e9da275c/e/b9028454f0634d679840eab5

    • Move face. The move face feature with the Rotate option is a great tool to rotate faces. Here I use a construction line created in the sketch to rotate the upper face of the cilinder 30º
    • Extrude 3 feature. This extrusion feature creates a surface instead of a solid part. If I try to create a solid extrusion the accuracy is worse and the cut of the slots would not be perpendicular to the cylinder. 
    Extrude in 2 directions:
    1- You can extrude a solid or surface in 2 opposite directions, like in this picture


    2- But if you change the second direction (flip the arrow Opposite direction) then instead of start from the sketch plane the extrusion strat from the difference of Depth 1 and Depth 2


    • Extrude 3 feature.(Continuation). So the extrude 3 feature use the above option to extrude up to the lower face of the cylinder from the upper face (the slopper one). To keep a separation of 10 mm with these faces, the offset option is activated and a distance of 10 mm is indicated.
    • Thicken feature. The thicken feature removes from the cylinder the solid created by giving thickness to the previous surface. To ensure that there are no problems it is assigned twice the thickness of the cylinder wall (if a thickness of 10 mm is indicated, the operation gives an error)
    • Circular pattern feature. The circular pattern of the features Extrusion 3, Thicken and Fillet is created with the option Apply per instance activated. So the rest of the surfaces instances are created, which are given thickness, removing them from the cylinder and rounding their edges.
    The surfaces created with the circular pattern have not been removed, they are hidden and you can make them visible again.

    If you uncheck the the option Apply per instance, the circular pattern just copy the geometry in each instance without recalculate them.

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  • lanalana Onshape Employees Posts: 313
    @larry_hawes
    Circular pattern dialog box refers to features it is going to pattern.

    Each feature defines its own behavior when patterned, I explained above how extrude behaves. So bounding face does not belong in pattern dialog, it is a part of extrude feature definition. Please try reading feature pattern documentation - it probably explains it better. Try using feature pattern - you'll get a better feel for it.
  • mahirmahir Member, Developers Posts: 794 ✭✭✭✭
    Elegant solution, @emagdalenaC2C
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