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The Fasten Mate - using created mate connecters

I am a recent user of Onshape  and learning about the sketching features , currently working on an assembly using geometric parts that I sketched; having a problem using the 
'Fastened mate ' to connect the rod to the frame. Is there a step that I am missing in the process? 

Would appreciate any help you can provide!

https://cad.onshape.com/documents/52fada1a7504bd0e82de5cd2/w/b6f854dbe230995041249519/e/e4ad49e6a43ee657feabc84c

Best Answer

  • billy2billy2 Member, OS Professional, Mentor, Developers, User Group Leader Posts: 1,640 PRO
    Accepted Answer
    @alison_gray769

    Have you ever thought about using a sketch to describe what this part studio is going to do?

    I'm thinking your 1st feature should be a sketch named layout and used as the skeleton for your design.

    Remember, you can import that layout sketch into an assembly and use it to assemble.

     The main benefit is for the next guy trying to understand what you're doing. It's hard to follow a bunch of parts and what their supposed to be & become.




Answers

  • wayne_sauderwayne_sauder Member Posts: 159 PRO
    @alison_gray769
     Your mate connectors that were added in the parts studio are a bit confusing as to your intent so I made some assumptions. 
    Is this what you had in mind? I only create mate connectors if the default connectors do not give me the position I need, or occasionally if I wish to speed up repetitive assembly. Most of the time I find I am able to get the position needed with the default mates and offsets. 

  • billy2billy2 Member, OS Professional, Mentor, Developers, User Group Leader Posts: 1,640 PRO
    Accepted Answer
    @alison_gray769

    Have you ever thought about using a sketch to describe what this part studio is going to do?

    I'm thinking your 1st feature should be a sketch named layout and used as the skeleton for your design.

    Remember, you can import that layout sketch into an assembly and use it to assemble.

     The main benefit is for the next guy trying to understand what you're doing. It's hard to follow a bunch of parts and what their supposed to be & become.




  • robert_scott_jr_robert_scott_jr_ Member Posts: 86 ✭✭

    "Have you ever thought about using a sketch to describe what this part studio is going to do?"

    This sounds as if it may be a useful tool. I apparently do not have the imagination to picture how it would work. Do you have a public document you can point to as an example? - Scotty

  • billy2billy2 Member, OS Professional, Mentor, Developers, User Group Leader Posts: 1,640 PRO
    Holy crap batman!

    Let me find one for you, there's a claw in the tutorials that expounds this concept.

    Onshape is a parametric modeler and it remembers everything you pick. So pick wisely.

    It's best to start simple and build your ideas up in logical steps. I believe you have an idea in your head and your trying to make a shaded 3D CAD model. You have all these parts that you've figured out in your mind, you drew them and now your trying to put them together. 

    That's really hard to do and it's not necessary. Let OS do it and capture the steps

    The other problem, for me, I don't know what's going on inside your head and it's important information. One thing that I preach, and I'm preaching how to build models with design intent. If your working with a guy who has an idea and wants to build a product, that napkin sketch is important especially if your filing for a patent. Capture it because you'll need it.

  • billy2billy2 Member, OS Professional, Mentor, Developers, User Group Leader Posts: 1,640 PRO
    edited November 11
    Ok, it's easier for me to create one.

    https://cad.onshape.com/documents/7fb41efc3e90820ffcb95eca/w/8538cad1400bf7739a959cb5/e/32b01c35f31df82e72354ec4

    Things to know:
    -I created the document above and made it public so you can access it. You'll have to make a copy of it. Most my work is private
    -The tab labeled "layout sketch" has the layout sketch example
    -Double click the "layout" sketch and then click on the final button
    -Hold the shift down and drag the sketch around

    What does these 3 links do? It obvious right.


  • bruce_williamsbruce_williams Member, Developers Posts: 810 PRO
    @billy2
    thanks for the 'lessons'!  Sorry this linkage use is not obvious to me.  Could you add an assembly please?
    www.accuratepattern.com
  • billy2billy2 Member, OS Professional, Mentor, Developers, User Group Leader Posts: 1,640 PRO
    edited November 13
    @bruce_williams


    Sure, let's go over everything.

    1st the link above has a "w" in it which means it's tied to my workspace and not to a version. Updating my document automatically updates the link. Actually the link is tied to my workspace in my document. For you to work on the updated document, you have to re-download and make another copy. You'll have to click the link above and make another copy. FYI, we've bitched about this, but it's a security issue. Anyone clicking the link gets the latest, but your old copy doesn't update.

    If there's a "w" in the address, then you'll always download the latest. If there's a "v" then it's stuck in time. That's the difference between a workspace & a version.

    Discussion points:
    -assemblies & part studios go hand & hand. You should never have a part studio without an assembly. Why? because there's things that are much easier to do in an assembly like assigning properties to parts.
    -the 4th link is the ground but the assembly has no ground. Who cares? I just imported the original layout sketch into the assembly and made it the 4th link.
    -if you open the assembly, I don't have all the links referenced to the sketch, instead I reference the links. This means the linkage can move independent of the sketch. Who wants to go to the part studio to move the assembly? The link lengths are associated to the sketch but not their location. Is this correct? It's my choice there is no right or wrong.
    -from the layout sketch, 1st feature is the tree, renamed something special, anyone can open it and understand what this document is going to do/be.
    -Let's talk about what you don't know. If I change the cyan link's thickness, the blue link updates.


    This is my design intent. It seems to me that these links should stay coplanar to the background. Design intent is illusive and hard to expose to the next user. Ask @pete_yodis, he loves it when an engineer sprinkles a lot magic to a model. Manufacturing doesn't want things to change but as a designer I want predictable change. Thus, parametric modelling. When I'm modelling, I'm thinking about the impending changes that could come along. If I'm right, then I can update my model during a design review meeting and my job is complete when the meeting ends. If not, I'll make a note and write the change down on a piece of paper. How do I know if the model will update? When using a parametric model you'll get a feel for how robust your design was constructed and what you should try to do during a meeting. Pretend you're demoing in front of a prospective customer trying to sell them something.

    Someone in the forum wished there was a place to add notes about a document and I thought this was genius. There's so much to a well constructed model and renaming sketches isn't enough. That doesn't mean use shouldn't do it. I look at a lot of people's models. Comment your code. I don't care how good you are, you ain't nothing if someone can't follow what you're doing. In more complex projects, you have to document your structures and how things are being put together. 

    I know you're an instructor, is this too much? Please teach the proper way to model. There's so much trash out there.



  • bruce_williamsbruce_williams Member, Developers Posts: 810 PRO
    @billy2
    OK!  that is a great example of some design intent and using the part studio for trial (moving the layout sketch around) and tying the linkages together for likely changes.

    When you said it is obvious what these three links do, I thought you meant in a mechanical purpose. You mean as a demo of changing the layout and having the linkages follow. Layout sketches are critical for driving design in a editable way.

    In order to drag the layout sketch vertices, it is necessary to leave it at least somewhat unconstrained. It is surprising that the down stream sketches (for linkages in this case) show they are fully constrained. That is SO COOL!

    You have some well thought out workflows and I am working to understand fully.  I will continue to look at your other recent posts. I think your in-context stuff is really good and I will have some questions in those threads.

    And this is not too much at all. I am sure many appreciate your experience and explanations.

    btw - I am just starting a second career of instructing so you are right on about setting the right direction.  My career has been more about one off tooling with assemblies of engineered components not much in my history.  Good to have the forum and Onshape support to understand this side of CAD.
    www.accuratepattern.com
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