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Amount of detail present in sections used in part modeling

F

Freecat

Member
I have read differing opinions regarding the amount of detail to include in a sketch used to create part geometry. I am wondering what other Pro-E users would recommend? I've been told to keep rounds and unecessary geometry out of the sketch, however I have also been told the opposite, to include those details in the sketch to keep the model tree feature count small, which in turn helps regeneration time.



Any suggestions?
 
My preference is to detail the heck out of sketches, and include rounds, chamfers and lead-ins.



One reason I detest intent manager.



Highly detailed sketches result in considerably fewer features overall which makes for:



smaller file sizes

easier troubleshooting,

shorter learning curves on unfamiliar models

faster regen

easier feature/model management overall.



One argument since time in-memorial for leaving rounds out is so that they can be suppressed for FEA. However sketches are easy to redefine too and modern meshers and computer processors can handle rounds more effectively.
 
Forgot, more detailled sketches also reduces the number of parent-child relationships..



Detailed sketches = easier life
 
Keep your sketches simple! They will be far more robust in the end. Don't worry about feature count. A dozen datum curves and a single protrusion will generate just as fast as a complex protrusion with the same end geometry. The advantage to keeping sketches simple is that they will be easier to control. You can also name indivitual datum curve features, thus being able to re-use them with use edge options for any feature that follows. Parent-child relationships are not bad, if you know how to use them to your advantage. Also, turn off that d**n Intent Manager! I can't do anything you can't do yourself!
 
What would you rather deal with - a 200 feature model or a 100 feature model ???



Feature count is a sadly overlooked metric of good modeling.



Granted datum-curves don't impact regen much but rounds, chamfers and other features do...
 
It sounds to me like the answer is a combination of both strategies. A more complex model with a predictably high feature count will more than likely benefit from highly detailed sketches, whereas a simpler model will not really benefit, and it may actually be a hinderance in the time it takes to create the model. With the aformentioned pros and cons of both methods, what do you think of the following sketching strategies:



More complex model = more detailed sketches

Less complex model = less detail in the sketches

Changing sketching strategies relative to model complexity= even easier life for everyone!



What do you think?
 
You're right, for simple models it probably doesn't matter one jot.



This looks a good strategy.



PS What would you consider a complex model ??
 
A motorcycle engine crankcase (high feature count of course), I work for an aftermarket motorcycle engine mfgr. I am currently learning Pro-E as our current CAD system does not deliver a complete engineering solution. Our current system is very easy to use, and it is a good software to produce a 3D CAD model, but it lacks the ability to be a complete engineering solution.
 
Including rounds in the sketch for simple and complicated parts may bring down the no. of features. But while making a casting model, which includes a no. of drafts, it is better not to sketch the fillets. No. of features is secondary. To make a draft is important.

Rajesh
 
Point is, it's different in every case. You should always take into consideration the design intent of the model. Think about what might need to change, and what is fundamental to the design. Then model for ease of revision, robustness, or whatever combination suits your design needs.



Generally I prefer complex sketches for the reason of easy manipulation. If I open a complex part with 100 features and I need to remove a surface, it's going to cause a number of failures in the children. If it is all sketched in as few features as possible I can just redefine the sketch and be done with it. No weeding through failed features, or UNDO CHANGES to see what went wrong. If your sharing files with other users, always take them into consideration. Everyone hates working on someone elses overly complex model!
 
How anyone can argue that feature count is secondary or irrelevant is beyond me.



The math is simple:



complexity (constant) = simple sketches * high feature count

complexity (constant) = complex sketches * low feature count





I'll take complicated sketches/low feature count any day...
 
Thanks everyone for the replies. I learn so much on this site, the things that you don't read in the books. I will keep these tips in mind.
 
I still reckon it's better to keep sketches simple when parts are complex.

I learnt this when I modelled intricate extrusions. The cross-sections had hundreds of small lines, all inter-related.

At first I modelled most of it in one protrusion. The regen time was horrendous...

As an experiment, I did another model with a simple protrusion, then simple cuts to remove material, then groups & mirrors/patterns of these cuts to create the extrusion surface. It regen'd in a fraction of the time.

Plus it was easier to change a size later. You just changed it once or twice & they all updated. When I opened sketcher with the original sketch, it took ages to display because of all the lines (and my workstation!)



As was said above: for simple parts (with less than 10 individual operations) - go ahead & model either way, it has less impact.

But for more complex parts, think ahead - the next person that comes to the model will probably thank you if it's easier to understand - with separate features for operations.



If you want to clean up your model tree - use groups. Group together features that are related by function or area. For example, group together a bunch of cuts & grooves used for a pipe end attachment, etc... A group collapses to one line in the moel tree, and can help to simplify the structure.

If you think about it, the model tree should be just that - a tree - with branches...
 
What regen time are you refering to ??



I have some horrendous sketcher regen times but usually once thru this stage the model regen times are exceptional.



Troubleshooting is a breeze as parent-child relationships are minimized and there are fewer features to track.



I would imagine extrusions don't have much in the way of children (some holes and cuts maybe ??), try modeling a complex casting with bosses, ribs, webs, draft and all the other stuff that goes along with them...
 
Do not make the sketch complicate, keep the sketch dimensions not more than 10, the more dimensions will make the regeneration time forever, and will face a lot hassel when redefine the feature.
 
Im curious if PTC has any info on regen speed comparison of sketcher complexity, i.e., rounds in a sketch vs. a separate feature.

My preference is to have the ability to suppress rounds, chamfers, drafts as an individual features.
 
That would be interesting but sketcher complexity has always been a taboo with PTC and have always found them to be immovable on the subject.



If they were able to flex they'd open up a bunch of serious marketing opportunities.



One thing I do know is the minimum of fetures is always good and not just from a regen standpoint but investigating & troubleshooting other people's models (actually including my own too)..
 
Dear Friend,



Keep the sketches simlpe in complex model & if possible remodel that with sketches with details included in.



you will find the best answer & will make ur own opinion

& I know what ur opinion will be.





Hrishi
 
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