Hybrid design v catii

[moi]

mogoce kdo ve, kaj je razlika med hybrid designom in navadnim?
ce sem prav razumel, naj bi bil HD nekako tako kot solidworks, kjer lahko modeliras s kombinacijo povrsin in solid partov, kakor ti pac zapase?
tisti, ki delate v automotive industry, kaj uporabljate, imate kaksna priporocila glede tega?

[M38885]

To vam ze sam naslov pove, Hybrid.
Drugace to v Auto-ind. ni dovoljeno uporabljati, ker je kljub vsej history Hybrid le "neumen element" v konstrukciji.
Priporocilo: izogibajte se ga.
Le ena uporaba je dovoljena: dobavitelju odlitkov je treba na hitro dostaviti Model (Informacijo) za njegovo kalkulacijo.

[moi]

kaj pa pomeni to potem? da so povrsine in solidi v istem drevesu al kako?
sem pa slisal ja, da v bmw recimo ne dovolijo tega, sicer podatek iz leta 2005.

[M38885]

To pomeni, da se Hybridov izogibajte in da tudi letu 2013 Hybridna konstrukcija v nemski Autoindustriji ni dovoljena.
Pravzaprav mi ni poznano, kje je dovoljena.

[moi]

lp,

sem si malo pogledal in izklopil hybrid design. hvala za nasvet.

tole sem našel. avtor je avtor večih kompleksnih tutorialov za catio (audi r8) in se vidi, da se spozna.

In catia, when starting a new part,you will be askedwhether Hybrid Design mode is on or off. Thisactually affects the tree structure only. For both modes, you can use surface & solid modelings together.


=========== Tree structure


If Hybrid OFF, solids will be stored in the folder "Part-body" while surfaces/curves will be in another folder "Geometrical set". On the tree, you can see both folders.


If Hybrid ON, solids/Curves/surfaces all will be stored in "part-body", which is like Solidworks


============ Parent Features Keep/ not Keep


Suppose i create an Extrude surface, then trim a hole on this surface....


If Hybrid OFF, we have two surfaces, the trimmed surface in SHOW area and the originaluntrimmed Extrude surface in NOSHOW area.


If Hybrid ON, we only have one surface, the trimmed surface. The original surface is "ABSORDBED", as Solidworks does


============ Features Grouping


If Hybrid OFF, all features in a Geometrical set can be moved into another Geometrical set anytime. The ordering is not important. It is useful to hide a group of features (maybe some surfaces with some curves)

If Hybrid ON, we cannot move a surface into a Geometrical set because the tree ordering is important. To hide a group of features,first define a "SELECTION SET" and then hide the selection set. This concept is like Layeringin UG/ Autocad.


============ Features Re-use


If Hybrid OFF, allparent surfaceswill be kept and can be found in NOSHOW area. We can re-usethem anytime


If Hybrid ON, first"ROLL BACK"the tree, justunder theparent surface, then "EXTRACT" it to duplicateone more for another feature.


==========Some comments


For simple models with little surface-modeling,both are ok;thetreewill beeasier to understand if Hybrid is ON. Solidworks enthusiasts may find easier to accept.


For complex models with lots of surfaces &curves, hybrid OFF is better. it is better for feature re-use & re-grouping.


CATIA is designed for everyone with different backgrounds and different design practices...

ni mi sicer jasno, za kaj je uporabno tisto premikanje featurov med razlicnimi geometric seti...

[CNC tehnologija]

Pozdravljeni,

Mene pa zanima, kako je v Catia podprto modeliranje solid teles glede na uvožene STL površine.
Primer:
skeniram 3D telo - dobim STL zapis scana, rezultat: lahko je odprta ali zaprta STL struktura.

Zanima me, če bi iz STL strukture lahko najprej "očistili obliko" in nato "zašili" končno 3D zaprto telo, ki bi se z boolean operacijami obnašalo kot vsako drugo klasično solid telo. Povdarek postopka je v temu, da pred šivanjem solid telesa ne narišemo nikakršnih krivulj in nobenih analitičnih površin preko STL strukture.

Ali je to možno v Catia ?

V našem primeru je potrebno hitro modelirati 3D telesa tako, da jih obrezujemo s odprtimi ali zaprtimi STL scan površinami/telesi. Podatki iz scanerja v našem primeru so bolj merodajni kot teoretični 3D model parta, saj pokažejo na dejansko zvijanje po ulivanju kosov.

Hvala za odgovor.

[CNC tehnologija]

Ok odgovor sem že dobil pri zastopniku.
Solid body lahko dobiš, če intenzivno delaš v modulu za rev. eng. Kar pa zahteva kar veliko dela...