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Best modelling practices

tinag

New member
Hello all,


After some recent problems caused by poor modelling methods i have been asked to design a sheet of best modelling practices, as at the minute we have no standards set out and some of the models i am being sent for manufacture are appallingly designed and almost impossible to modify or change.


Does anyone use such standards, or have any suggestions where to start ? I know alot of it is just common sense... something which seems to be lacking in our design department
..


TIA


TinaG
 

dr_gallup

Moderator
You might want to look into Delphi's Horizontal Modeling techniques. They basically limit the number of dependancies to as few as possible and make the sure all references are to base datums & features. The goals are to make robust, easily modifiable models. I swear they copied my SOP.
 

paulcunningham3

New member
Yes im seen them and the are quite good i strongly recommend that u use modelcheck to set up your proposed standards and check your models are abiding by them. Get active maintenance for full access to ptc tutorials remember these guys designed the software!! so quite frankly know best


Paul
 

tinag

New member
Thanks for your responses... Unfortunately maintenance is not an expense which this company likes to consider.. when they want to upgrade they find it cheaper just to purchase new licenses. The standards are to try and stop bad modelling habits, some of the designers here have been using proe since it was pro junior ! Ive been using proe for 6 yrs. Using model check is ok but i need them to create useable / modifiable models first time instead of me having to re-draw them every time a part needs modifying or manufacturing. I need to give them a "kick up the Ass" with their modelling techniques.. but unfortunatley physical violence is not an option
,though it would probably work best.


They all know the basics to modelling, but i need to find a way of getting this need of correct modelling practises across (without any ass kicking), hence im trying to right some guidelines for creating new models.


TinaG
 

AHA-D

New member
A lot can be written on modelling techniques. The thing mentioned above of attaching as much as possible to base datums and base features is certainly true.


One other thing is "keep it simple". Some of the old designs (turned parts) I open here have profiles that include all the details, roundings and chamfers included. To me that's poor modelling. You can't find the dimension you need to change in the number-cluttered screen, and when you do find and edit a parameter there is no way you can predict what will happen. It may be nice to have a feature tree with only 10 lines but it doesn't make it more manageable.


I'm much in favour of modelling according to fabrication steps. If you have a turned part this will be cut in discrete steps, it's (IMHO) best if these steps can be found in the model. Meaning grooves, rounds and chamfers are separate features and not embedded in any major profile.


If one feature is dependent of another I prefer to model it that way. This may sound contrary to the first rule of attaching to base datums, but still makes sense. Say you have a cilinder diameter 10 in which you need a groove reducing it locally to 8. One way of dimensioning the cutting profile is to make the outer limitlarger than 10, say 12. As long as your cilinder has a diameter below 12 the feature will hold, but beyond that you'll find yourself with an invisible revolved cutout. Locking the cutout to the edge of the cilinder makes it dimensionally totally independent, although you're now bound by a dependency between cilinder face and cutout.


Alex
 

dr_gallup

Moderator
Rounds and chamfers should be created as separate features and as late as possible to avoid referencing them. this also makes it easy to de-feature the model for FEA or simplified reps.

I definately prefer multiple features with simple sections over a single complex feature. It makes redefining a section much easier. I try to follow machining steps as we frequently make process sheet drawings from our models. So if we drill, ream & grind a hole I make that 3 features although it could be one. They will all reference a common axis. They do not reference each other so the order can be changed or one deleted without affecting the others.

I'm a big believer in using the part dimensions (shown dimensions) in the drawing, but many hold opposing views. Check out this post for some strong opinions on the subject.
Edited by: dr_gallup
 

paulcunningham3

New member
i totally agree with dr gallup u need to think about what your making in have many colleague who make complex features with loads of unneccesary constraints which make modifications simply a nightmare, but at the same time I wouldn't reccomend using to many feature to define parts or efficiency of modifications will suffer so a happy medium must be reached!


And I agree that ptc dont ALWAYS know best! lol





Paul
 

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