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Good modeling practice.

Or should we be building draft into sketches as well? :)



You can if you think it's appropriate for your design intent.



In SolidWorks you can also specify draft as an inclusive part of an extrusion and not as a separate feature:



View attachment 335



Isn't this cool, now why couldn't PTC do this ??



I work both Pro/E and SolidWorks and IMHO SolidWorks guys understand user needs way better than the PTC guys. (check some of the previous replies in this thread for a case in point).





:)
 
Right from the SolidWorks documentation, it says, Sketched fillets can be recalculated much faster than fillet features, but complex sketches can be harder to create and edit.



I think that illustrates my point completely.



Faster regeneration is not the priority in good modeling practices in Pro Engineer. Creating a model that is as robust, parametric, and associative as possible is the goal.



Good modeling practices in one CAD system simply aren't going to be the same in another CAD system. SolidWorks and Pro Engineer are aimed at two different sectors of the market (mid vs. high end).



And if having worked for PTC and continuing to consult for PTC is a liability when discussing good modeling practices in Pro Engineer, then I'm guilty.



David Martin

Torgon Industries
 
If I remember this is forum for PTC users, and not for some fanny guys which using Solid Works! If you think that SW is better, than go to some SW forum. Ok





Speling
 
One question

Why using SW, when ProE can do the same and much more? That is my main question.

Why you not use ProE when you buy it (did you), and use another packages (SW) paying it (will you), with all imperfection it have etc





I forget to write this regarding above mentioned learning processes



I have my own process and ideas for learning people how to use ProE. Much more than only few times that process has been proved like very productive and easy to understand and implement. I must admit that from classes in PTC and my classes exists one big difference.



I teach people how to work in the Field of Industrial Design using ProE like best solution for modelling
 
Faster regeneration is not the priority in good modeling practices in Pro Engineer.



Maybe, if your dealing with a 1000 feature model it sure can be...



Creating a model that is as robust, parametric, and associative as possible is the goal.



No, No, No.



This may break your heart and rock your world but this is only a SECONDARY goal.



The PRIMARY goal is to model actual, finished parts as accurately and as representative as possible and this means right down to dimensioning schemes and tolerances.



If this means a model is not quite as robust as it could be then so be it - get over it !!!



Do you seriously believe that nice Pro/E models are more important than the actual parts that they represent ??



Good modeling practices in one CAD system simply aren't going to be the same in another CAD system.



Modeling for design intent never varies from one system to another or one company to another or one country to another..
 
Doug, as I said earlier, I am limiting my discussion strictly to modeling, not part design. Therefore my comments refer only to CAD side of the process. Are Pro E models more important than the parts they represent? Of course not. But my comments refer only to CAD for the sake of discussion.



And good MODELING practice certainly varies from one CAD system to another. Perfect example: filling in holes you no longer want with protrusions / solid material. In Boolean operator based systems, this method can be acceptable. In feature based parametric modelers, this is very bad. Good design does not vary. But again, for the sake of discussion, I'm limiting my comments strictly to CAD aspects in Pro Engineer.
 
I am limiting my discussion strictly to modeling, not part design.



You are implying that modeling and part design are mutually exclusive - they are not.



Aren't models (any model, computer generated, carved from stone or whatever) intended to be representative of the part ???
 
All,

My 2 cents....

All of the good modeling practices were clouded by the tit-for-tat of rounds. There are many GOOD modeling practices but BEST modeling practices are a misnomer. What is best for one design or industry may not be BEST for another. Your design intent and manufacturing techniques should be the driving factor in all designs. The sign of a good model is first and formost it's ability to convey the manufacturing data required to produce it. That in turn menas that to have a model near to perfection, the Design Intent, or the way in which the engineer wants it react to changes in dimensions, should closely match the capabilities of the process by which it is produced. They hardly ever do. Why? Most engineers are not aware or trained in manufacturing techniques and processes. It takes a designer with both engineering and manufacturing backgrounds to produce a robust, correctly dimensioned, correctly tolereanced part and drawing. ....

So as for rounds. IMHO, and experince from , engineering and manufacturing design projects.

1) Add them as late as possible. They tend to get used as references accidentally by most everyone making it near impossible to change or delete later.

2) Add rounds as separate features. Rounds are FREQUENTLY changed or removed. They are changed from rounds to chamfers, or from radius to elliptical, or from constant to variable. As a separate feature they are much easier to change and delete without affecting later features. Try changing a radius round in a sketch to a variable radius round. Redefining sketches is the last resort in changing something because your design intent should have included the possibility that the rounds might change and adding or removing sketched entites is one of the quickest ways to break P/C relationships. Many users either don't know how or are not properly trained in reroute, replace, or resolve mode so making it necessary to do so is poor modeling technique.

NONE of this means that you should NEVER do it, but that NOT doing it in a sketch is PREFERABLE if possible. I have inherited FAR TOO MANY models that took days to fix instead of minutes because of rounds included in sketches or used as references.
 
OK- now for my good modeling techniques.

2 cents more but not all inclusive.

1) Use your head. It's the best tool you have. Think first, then model.

2)Think about how the design may change as the project evolves and build in that ability.

3)The number of features used is irrelevant.

4)Your model SHOULD have > 95% dimensions SHOWN. The drawing should reflect both the design intent and manufacturing needs.

5) Use patterns when possible.

6) use HOLES when making holes, and cuts when making cuts. The cut may be round today but may be oblong or slotted tomorrow. What you thought was a hole was really a cut.

7)Think like a mchinist when creating machined parts. It makes the design easy to follow and understand.If you don't know hat processes or steps might be used to create your part, ASK, someone knows.

8)Dimension and tolerance your part using GDT and expect manufacturing to need help deciphering the symbols. FEW people, engineers or machinists, really understand GDT.

9) Don't delete and remake similar features. Try redefining first.

10) Use Parent/Child references to your advantage. Don't just pick willy nilly when creating features. Uae query select to ensure you have selected the correct parent for your feature.

11) Use relations to create design intent such as preventing a redius from becoming to small or to big.Make sure you comment your relations.

12)Don't save or submit models with suppressed features.

13)Name features so they can be logically understood such as Parting surface.

14)Use company standard start parts with all appropriate pareameters included.

15) Check for and remove geom checks

16) Use model check (comes with Pro/E) to find other geometry related problems like very small edges.

17) Pro/E is NOT boolean, never fill a hole or void with a protrusion. Redefinr the offending feature to fill it in.Why? Some day down the road you make delete that second protrusion exposing ahole never meant to be there but you forgot or a new user never noticed it.

18) make sketches simple. Complex sketches are a pain to constrain correctly and then like rounds, individual features in that sketch may need to be deleted later requiring you to redefine your sketch and then replace, reroute, or redefine other entities or features. PTC says 12 enties is about right. I think thats arbitrary but a seasoned user knows when there are just too many entites. A lot of entites also cause regen problems. Try selecting text edges of a previous feature while in a sketch.

19) check your accuracy. If creating assemblies of vastly different parts you may want to use absolute accuacy. The same goes for units.

20) assign material properties. This gives correct mass props for CG etc.

21) Learn a little about stress and strain. Don't design parts doomed to failure by using bad geometry. Know your requirements for stress, vibe, etc. This also makes the liklihood of large geometric changes smaller in the future.

22) When designing in a concurrent engineering environment, be able to create shrinkwrap parts or envelope parts from your model for use in upper level assemblies. If you create bad geometry at the part level it makes creating lightweight parts harder.

23) Don't use exteranl references unless you absolutley have too.

24) I'm tired so i'll end with GET SOME TRAINING! Particularly if you are using specialized modules like cabling or piping. You may be getting by today but later on the models will turn out to be the bane of your exixtence and cause huge delays in your program because you didn't understand the repercussions in your design choices.
 
Someone turn a hose on these guys ! :)



Why don't you turn a hose on yourself :)-8 :), this is a significant issue, the argument is:



Do we model to meet design intent and make them as representative of actual parts as possible or do we model just to make nice models ???
 
I would like to add one more point. Frequently, I need to make process drawings which show the part at each stage of the manufacturing pipeline. Therefor, I tend to make very simple features for each machine tool used. So if a bore gets a pilot drill, finish drill, ream & chamfer I make that as 4 features even though a single revolved cut could do the same thing. That way I can have an instance of the part at every step to make inspection drawings. Also, if the manufacturing engineer wants to change the order of the chamfer and the ream I just reorder the features. I try to make every feature independant of the others even though this requires lots of closed sections which PTC recommends against. I find that closed sections are much more robust.
 
Actually, PTC does not recommend against using closed sections. Almost the opposite. The company line is, choose between open and closed sections depending on your design intent, but when in doubt, choose a CLOSED section because they are more robust.
 
In engineering, unlike philosophy or theology, pragmatic considerations are really the only ones that matter. The only thing that matters is this: What get the results needed at the least cost. That question can be harder to answer than a philosophical one, however.



I disagree with some of what has been stated as good design practices and I offer a few of my practices for consideration and criticism.



To start, jabbadeus gave this proposition:



~



4)Your model SHOULD have > 95% dimensions SHOWN. The drawing should reflect both the design intent and manufacturing needs.



~



Assuming he means your DRAWING should have > 95% of the dimensions as SHOWN dimensions, I would say this statement is restrictively dogmatic. Shown dimensioning is a nifty idea that has very little practical use, IMHO.



I would hate to have to be concerned with how I dimension my sketches because of how they might appear in my drawing. What an unnecessary burden and restraint on flexiblility! What happens when I get to my drawing and realize my feature dimension isn't really suited for my drawing dimension. Now what? Am I going to go back and redefine my feature so that my shown dimension is the way I want it, or just create the dimension I need (which I could have done just as quickly in the first place)?



Another problem with using shown dimensions is that assembly feature dimensions can not be shown in a view of a part model. Only part feature dimension can be shown in a part model drawing. Should I give up the power of assembly features so that I can use shown dimensions? Why would I give up such a productive capability for something that doesn't even save time?



The second part of this principle is a great sounding idea:



The drawing should reflect both the design intent and manufacturing needs



but is in fact is just as impractical as the first. I agree the MODEL should reflect both the design intent and manufacturing needs as much as is practical, but for the drawings, its pointless.



This is why:



We are a manufacturer of plastic injection molds. We build from 3D data (ProE models about half of the time). We



don't see our customers prints until we are through building their parts! Therefore, any effort to reflect anything other than inspectional requirements is an absolute waste of time (and obviously we don't need them to build the tooling).



Why don't we have prints to reference in the manufacturing process? Probably because, practically, it is not that vital (at least if you have a good manufacturing partner). Product designers, like manufacturers, have there backs against the wall because of time constraints (for the product designers, its because they spend to much time playing golf). Because of the compressed nature of the design and build cycle, manufacturing begins DURING the design process, and is typically completed BEFORE the design process is completed (if you include producing drawings as part of the design process) Typically from our experience, by the time product designers find time for making prints, the only process left is inpection, and often times we have to wait for prints for inspection!



Product designers need to realize this so that they will stop using drawing-dependent anomalies like offset tolerances (non-symetrical tolerances like +.005/-.000) that cannot be maintained by building to a 3D model.



Except for the simplest assemblies or parts that are not used in assemblies, it is illogical to drive models from drawings. What is the purpose? The only purpose I see is to enable someone unfamiliar with the model to be able to make changes to it from the drawing, but that person probably shouldn't be changing the model anyway, since they wouldn't know what affect it might have on other features.



Does any one else find using shown dimensions a useless concept? Does anyone else see drawings/prints approaching obsolescence in the reality of the manufacturing world?



I would like to discuss assembly features (which jabbadeus mentioned, also) next.
 
rcamp: It may be impractical for you to dimension your model properlly because of your unique manufaturing capabillity. How ever there are many of us who need to document the the part and assy's on paper. that is why I have told my people to develop their models with the proper dimensioning scheme
 
I instruct my people to use correct dimensioning scheme too.



The two primary functions of an Engineering Drawing are to convey all the necessary information to inspect a part and for manufacturing to derive their required information.



Dimensioning scheme is critical to convey information on set-up for inspection and to control tolerance stack-ups.



If correct dimensioning scheme is NOT used in models then you will always have to rely on Engineering Drawings to convey all of the necessary inspection information.



View attachment 336



If we can convey all of the necessary information in a part/assembly model then we have a shot at being able to eliminate drawings...
 
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