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WHY fully define a sketch?
Dave_Accardi
Member Posts: 2 EDU
I understand that defining the shape and size of a part is important, but why does a constraint with the origin (and orientation) matter? Does it come down to how something like a 3D printer will interpret the model?
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billy2
Member, OS Professional, Mentor, Developers, User Group Leader Posts: 2,014 PRO
Datums. Eventually you'll need to insure quality for manufacturing of your part and the origin + 3 planes are important features have for these operations. Also, the planes help with symmetry in many other commands. Having your design aligned with the origin is a good practice.
Way down the road you might begin to design based on datums vs. just adding features. This is the beginning of 'top down' design and offers more control over your parametric model.
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john_mcclary
Member, Developers Posts: 3,898 PRO
it's all about editing and making sure nothing moves without you telling it to.
You want to have full control of your sketch at all times.
If you change something else that has related geometry, then you can be modifying parts you did not intend to without any knowledge you did anything wrong.6
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Way down the road you might begin to design based on datums vs. just adding features. This is the beginning of 'top down' design and offers more control over your parametric model.
You want to have full control of your sketch at all times.
If you change something else that has related geometry, then you can be modifying parts you did not intend to without any knowledge you did anything wrong.
https://www.onshape.com/videos/sketch-constraints
'Datum' is just a point that all dimentions are measured from.
I have many sketches that don't have a single dimension as everything already exists somewhere else in the design to reuse.
In general: When a student has some blue entities in a sketch I will teach him how not to do it. If it is a professional engineer, he will owe me a beer
Only exception: Mirror construction lines without start or end.
Onshape has a couple videos on what constraints are and there a couple of posts here suggesting a strategy (few dimensions etc.) that are appreciated by newer users, but I can't find any real resource that outlines those strategies in a clear and cogent fashion. Is there a resource one might recommend other than an OnShape video that only illustrates what a constraint is and what it does?
Thanks in advance
Lemme ask a question first - are you guys basically trying to hand-draw your sketches to exact size initially as you would with something like tinkercad or sketchup? In other words if you know you need a 1" circle are trying to drag it to exactly 1" as you draw it?
I think the answer to your question, for me, is yes, though OnShape allows to set the dim as the circle is drawn, I would drag the circle left click, enter the dim, and click enter to define the dim. I can see that if for instance a center point circle is drawn starting at the origin, then dimensioned, the circle is fully defined . That same circle drawn in free space, then dimensioned, is not fully defined. This could be a perfect example of the best way to fully define that circle in free space. More than one method surely but those kind of defining strategies is what I'm curious about.
It is something you well get a feel for after a few years.
Don't worry so much about it now. but learn from your experiences. You will need to always be aware of "design intent" in order to constrain properly.
And there are always a hand full of ways to constrain the same sketch. There is no wrong answer, just some are more efficient than others to edit.
You will find some people will do it in different ways also.
You need to do what is comfortable to you.
And trust me, you may think you did it perfect. But then someone want's to stretch this end of the part in a way you never considered, and you well end up re-constraining it later.
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All I'm saying is make a conscious effort to stay on top of the possible changes coming down the line, and you will be just fine.
You can have no dimensions and all blue sketches (how it was in autocad...) Heck my first 3D cad assemblies didn't even have mates...
Maybe a course from our learning center will be more helpful than just the videos:
https://learn.onshape.com/courses/fundamentals-sketching
One of the sections of that course is all about constraints.
To answer another one of your curiosities, there is no one canonical way to define the location of your center point circle. The way that you define the location of your sketch circle in space is all just design intent. Here are a couple examples.
Maybe I want to define my circle as x and y distances from the origin:
Maybe I want to define the location of my circle as a distance from the origin, and an angle off the y axis:
In any case, the goal of our sketching system is that you should be able to directly portray your thought process about the location of the circle as a set of dimensions and constraints.
Watched the video (more than once) and understand 'how' to constrain a sketch, it's the 'why' that has me confused and will probably not be fully understood until I get more experience. The advice from posts above imply there may be better ways to define a sketch than others, perhaps more efficient, perhaps more flexible for future sketching/assembly etc.
It would be nice to have a resource of sorts that explained different strategies and why i.e. when to use dimensions and why; when to use const. lines and why; when to dimension to the origin and why; when to use tangents and why; or when to just use the blue lines because it suits one's purpose in that case.
I do understand I am asking something similar to, "What's better, dimension constraints or origin constraints," and there is no single answer but there may be a time and place where one is preferred over the other and with good reason. It's that 'good reason' that I can't seem to find a resource for.
I will certainly stumble upon my own good reasons to use one strategy over another but a resource explaining the reasons for a certain strategy might be helpful for beginners.
I have used it like once for something very temporary, I too have learned by mistakes to always 'lock' things in place for better control. And I try to avoid over-constraining stuff 'just t be sure' for easy editing by deleting the most obvious single constraint.
I think Onshape has pretty nice set of constraints these days and once you get hang of them, also editing and removing the right constraint is pretty straight forward.
Things can get very funny if you try to be smarter than cad and predict where it moves stuff if you give it too much options and it can be a pain to modify if you un-necessarily over-constraint stuff.
fixed references to external geometry?
That should use constraints or "use".
Fix is for locking something in place in the context of that sketch, so if you move the related object, your fixed point will remain relative to the origin of the sketch.
Sorry, I meant external geometry should be projected in the current sketch and then "fix" applied to it.
I donno, to me fixed is one of those "to be avoided" constraints.
I rather see construction geometry that visually explains how a sketch is defined.
This makes it a little cluttered sometimes, but anyone who follows you should be able to tell in an instant how a sketch will behave when they apply an update.
Consider the following:
This is a weird example, but what you can see exactly what position each circle will be in, and their diameters, without needing to mouse over and view relations one at a time. Fix is just another one of those you can only see it you mouseover the points, or turn on all relations.
Question here is, where did I use "fixed" below.. and why is it bad?
Answer:
The origin is not referenced, it is in fact floating by just a slight amount.
That is bad if you are using the origin or part planes/axis in an assembly. (mate connector in onshape)
your part will be off slightly enough to have mate errors in an assembly. Good luck to the schmuck who has to clean up after this hidden gem.
Fixed is evil if abused. Use it as little as possible to not at all IMHO.
I'll review as soon as possible.
IR for AS/NZS 1100
That's about the only time I can recall using fix, locking an imported jpeg centered to the origin and properly scaled. To do it with absolute dimensions would be trivial, as they would be random 6 place decimals that have not meaning to anyone anyways. I still throw one dimension on the image so I can copy and paste that in the same sketch on another plane.
Your simple 1st post ignited quite the discussion about the basics of parametric modeling.
I can hardly wait for your 2nd post.
I think most people starting out are happy to get geometry that looks right. After that, we all start building robust geometry that'll accept and build any change that could possibly occur. There's many techniques, all discussed here nicely and it takes time learning what builds robust geometry and what doesn't.
Trying to build robust geometry, you'll never get it perfect, solids fail. Some handle changes better than others and some are built in a way that is easy to understand & fix when they fail. Ultimately this is where you want to be.
I've always thought the best models are: visually correct, robust & easy for the next guy to understand. This takes time and it's what we're all after.
Welcome to the world of featured based parametric modeling and good luck! It's fun.