I agree with your manager, once you start fully defining everything you find it extremely easy to do (read "you find the work around's SW makes you do")
Some engineers link part sketches to external (other) parts in an assembly (IMHO, a bad practice). Some one goes in and changes the "external" part and the original part changes due to this, if the original part is used in other assemblies it will no longer "fit" them. Having all your parts fully defined can help eliminate that problem.
This is really an opinion based question. This depends on the types of models you create.
In my 11 years of using SW I have designed machined parts, casting parts, plastic molded parts,
sheet metal parts as well as weldment parts. Now with that said, the machine parts, sheet
metal parts and weldment parts I think it is fair to say that there is no reason for them not
to be fully defined. When it came to the casting and plastic molded parts (and I will throw in
imported parts as well) those dealt a lot with sweeps and surfacing and that is almost next to
impossible to fully define.
Because like you said Tim, the time wasted trying to place incidental dimensions to accomplish
that in my mind is totally ridiculous.
With all of that said, I am also the type of designer that try's to define my sketches fully
95% of the time because I like the dimensions in the sketches to be defined on my drawings
through insert model items.
As far as your manager? Forgive me but he sounds like a bit of a control freak. I think it
is a waste of engineering time and money to baby sit models to see if they are fully defined or not
as a criteria on whether or not they go into the vault. That basically is also throwing out engineering
dollars because if these parts are not important enough to be in the vault and be put into risk of being
lost that makes no sense at all either!!!!
Now, I also believe that with all the ways that parts are created, sometimes it is important to have fully
defined sketches because like Chris said, with parts depending on other parts in assemblies I have seen
it where one part gets changed and all of a sudden your assembly has errors because some relation
in another part was depended on the part that changed and because it was not fully defined, it made
some skewed shape.
Tim I hope this helped you and I think it might be a good idea for your manager reads this thread.
Unless you feel your job is on the line then maybe best he didn't.
Good luck with this.
Thanks, I appreciate the reply.
I argue this both ways. To me it depends on why you are leaving things undefined.
If you just skip dimensions because you're lazy, then I totally agree with the mgr. Simple line sketches should be fully defined. Then again, if you fully define things by just auto-dimensioning everything, and not using sketch relations, then that's a problem too. If you are dimensioning the endponts of centerlines, that's crazy.
I don't dimension sketches if the sketch is just an eye-ball job to begin with. If it is engineered geometry, then dimensions ought to be there. If it is just visual, or just splines, I don't bother.
Aside from working with simply visual models, I don't think there's a good argument in favor of leaving stuff undefined if you are doing real production work. But at the same time using the wrong scheme to fully define a sketch is at least as bad as not defining it at all. How the dimensions attach and behave during changes is as much design intent as sketch relations, so I think they are important. You won't see a best practice list anywhere that suggests that it is a "good idea" to leave sketches under defined.
I agree with most of that, but isn't it the resulting part that really matters? I agree fully defining a sketch is important i am not arguing that it is not. But, If the part functions as needed, does it really matter if you can go back into the sketch and one radius is not defined?
As a drafter designer who eventually inherits all of the designs and models created here, I can tell you that in my opinion they should not only be fully defined but also properly defined in the features things are located from. Nothing worse then going in to change the location of a feature and having some unrelated feature move because it was convienient to locate something from or to it. These types of accidental changes are easy to go unnoticed until you get the part back from the machine shop and it doesn't fit.
I'll second the part about properly related to other model geometry. I teach SolidWorks at a Technical College as a second job, and tell my students they must capture the proper "Design Intent" by using proper relations and dimension. And the fully defined concept is critical not only for the part being designed, but for any conceivable member of a "family of parts". That is just as big a reason and "inheriting the design" from another user.
There are some areas where I will let an under-defined sketch through in my designs. Sheet metal for one. If I create an edge flange, and enter the flange length in the property manager window, the created sketch is under-defined. I usually leave that. I guess I break a few of my own rules.
Fully defined assembly, correct? I agree
No, fully defined parts
Lots of good comments I am not going to repeat what others have said why everything should be fully defined
Is your manager anal?
management is about control (at least that's what most think and do)
Perhaps his rule is a reaction to too many sloppy parts and assemblies (parts and assemblies that are not fully defined)
An occasional one that is not fully defined, there may be a good reason it wasn't, is fine especially when it takes less than one hand to count the people compared to a larger organization
But when it gets to the point where the modus operandi is to not fully define ... well that's just sloppy/lazy/ignorant engineering
No two ways about it
Only to the person who may eventually inherit this part and be told to use it to create a new part "like" this one, but with some changes.
A radius being under defined may not cause headaches in the future, but other items may.
For your radius example (here I assume you are talking about a simple filleted edge or some such...) , typically this fillet is a 90 degree arc (1/4 of a circle). If this arc isn't tangent to the hroizontal and vertical lines it is attached to, this could cause issues.
1st picture, the arc is tangent, but not 90 degrees. 2nd. picture, same arc after someone changes a simple dimension.
Just some thoughts. Make it bomb proof and it won't explode.
I agree with this too, but this radius is easily defined, sometimes things are not so easily define-able.
Tim R wrote:
... but isn't it the resulting part that really matters?..
That's a philosophy that works for direct editing software, not for history based software. History based modeling is all about how you get to the resulting part. The main thing I try to consider is "how is someone else going to edit this part?"
does it really matter if you can go back into the sketch and one radius is not defined?
That's an unfortunate example. Radiuses in sketches are probably the worst offender when it comes to stuff that misbehaves when being changed. Also, there's the question of what you mean by "function". If the part has the right shape and size and features, that's one thing. But "function" can also mean how it reacts to changes. I mean unless you're the kind of guy who always models everything right the first time and nothing ever changes... and I don't think I know anyone like that.
Fully defined, whithout a doubt. Why? Because if someone goes back to your work at a later date, they can grab anything undefined in any sketch and drag it around, losing the integrity of the model. If it is fully defined, by you, then there is true intent and reasoning that goes behind it and stays with it.
I agree on the defining sketches in an appropriate way. It would be easy to just whack dimensions everywhere, but fully defining properly takes a lot of time which means a lot more money.
I define case by case. I have had the problem of wrongly placed relations coming back to bite me in multibody parts and assemblies, but in general not everything needs to be defined in the work I do. I'm really glad I don't have a boss like that. I repost direct to our GM though, so it's different.
After reading this I'm seriously considering stepping up my game though. Something to do when I have some down time.
As previously mentioned, this is an opinion based question. My opinion is yes, they should be fully defined. That's how it is in my world, though. I do 99% mechanical design, very little "swoopy" things so I'm not fighting with splines or other fluid shapes very often. By fully defining my sketches, it's my belief that my design intent will be apparent to whomever comes along after me to modify the part. That's my hope anyway.
Tools -> Dimensions -> Fully Define Sketch
I use this when I need to lock down a sketch and don't care how. If something can accidentaly move it will...
I'm from the pretty much unswoopy would, no splines in any of my models, but I do some castings.
All of my sketches are fully defined. But, I'm probably close to a control freak. I don't want someone to be able to go into one of my models, grab a blue sketch segment, and just drag it how they see fit. If it's going to be modified, I want it to be modified by changing something intently, whether it is just a dimension, sketch relation, or rebuilding part of the sketch. I can't watch over everyone's should, though.
How about this, once a mold/tool/die is made, isn't it fully defined? Don't you want to know your model matches this, to the best of your ability? Does fully defining your sketches help this, or are we now talking document control?
Sketches with just arcs and lines, I fully define. Splines are another story. You can have a spline that says it is fully defined, but it may not really be. You also have to constrain the handles to really have it fully defined.
I also do not use Instant 3D, to easy to accidently change a model.
VERY IMPORTANT. Unless you want geometry to change without your knowledge, they need to be fully defined whenever possible, which is all the time. The only way you would not fully define a sketch was if you were doing "recreational" modeling or something. But seriously you have been screwing up the kool-aid for the past 5 years.
I would fall into the “Fully Defined” camp. I find it rare when I find it difficult to fully define a sketch (I even dimension the control points on my splines). In a related thought… I have found it important to name my features. Not so much for the part creation, but when I need to go back 3 months (or days) later and make changes. The additional time to name them is more than made up while sorting things out during editing.
I've had to make changes to parts that were created by someone else using sketches that were not always fully defined...NIGHTMARE! I have a huge personal pet peeve on this issue as a result. Make one change and something else goes to pot just because someone was too lazy to add the proper constraints & dimensions. Unconstrained sketches can...have...and will bite people in the butt. Might be you, might be someone else, but it will happen.
I agree with Scott M. word for word. Its best practice to fully define sketches. I teach this to my SW Usergroup. Laziness is the only reason people don't fully define things. And that laziness cause problem on down the road. Especially if anyone has to work behind you.
I am the same way about Mates on parts, all parts in an assy should be fully mated. I only allow one exception and that's round fasteners, only two (they can rotate).
Always fully define your sketches.
Being able to edit by another engineer is a priority for us. I would even like to see more construction lines rather then only relationships so it easy for the next guy to figure out how the sketch is tied down.
I don't work with alot of complex curves so I can only guess at the problems it causes.
I don't do this but you can use "Fix" for those you can't define any other way. You will be fully defined.
Fully defined is best practice. Your standard should be that there needs to be a compelling reason for not fully defining a sketch.
I had a similar argument years ago with a designer using 2D AutoCad. He would not use snaps or ortho. Until I transferred him to another department, I would spend as much time marking up his drawings as it took him draw them.
I have always stated that fully defined sketches should be the goal but not the requirement. However, I think fully defined is THE way to go.
Good post; good feedback here. But in most technical scenarios (like engineering and designing) it is more important to know (and document it if possible) why you do something. In this case you should know why you work to fully define a sketch or why you allow it to be under defined.
Engineering is rarely an absolute, but most often an effort to be effective, which also requires definition or priorities for trade-offs and intent.
Final thought: if you require fully defined sketches then you may preclude yourself from using some SW features that are useful but still being developed, like 3D sketch points, which may require too much effort to fully define. It might be overkill and cost too much time, which could justify leaving them as under defined. Deciding and knowing why you made that decision is just as important, and in my opinion more important than blanket requirements. In SW having an under defined sketch should be a rare exception; it is usually so easy to fully define your sketches.
That's pretty close to my feelings about it, too