Does anybody use this modeling technique? if so any comments?
Does anybody use this modeling technique? if so any comments?
Sounds very promising, but it doesn't explain what the method actually is.. or do you have to take a course for it? and not able to tell anyone elsE? hehe.. i'd love to have more info on it, as we're struggling with different modeling method right now at work.. I'd love to find a more efficient way to make changes after the fact like discussed in the article.
Sent you a PDF that goes into more details.
Basic concept..... Do you model with a long, skinny feature dependancy tree (vertical) or a wide, flat feature dependancy tree (horizontal). I know that this has been discussed on this forum in the last few years at some point.
Nothing particularly new, but is an interesting concept that I beleive has a ton of merit.
Go get yourself a copy of xsi, it has built in tutorials, all geared around "skeleton" modeling. Then you can use those skills in the other cad/cam products you have.
It's modeling without your main features being tied to each other, hence the term (feature in-dependent) It is dependent on something though, usually a sketch, plane or another part. Here's a .pdf that describes Delphi's process.
Horizontal Modeling is just one word for it, you may also know it as Skeleton Modeling, Tier modeling, Sketch Assembly modeling, CAD Neutral Modeling, or Body Modeling.
Usually Jon when you are taking lessons from a company in Bankruptcy Court since 2005 its what not to do.
Usually Jon when you recommend company's follow the lead of another you shouldn't be recommending they follow a company removed from the NY Stock Exchange in 2005 and still in Bankruptcy since 2005.
I have been using this method for complex parts since 1999. These guys just coined the term. Were SW falls short is in having a feature tree in which it is hard to see whether you are working horizontally or vertically. There are addins for SW that allow users to see whether they are using horizontal or vertical modeling. You can also use the highly under-utilized parent/child menu pick to assess methodology. Even starting a delete operation and not finishing it will give a quick list of dependencies and give insight. That being said it is still difficult in SW to do pure horizontal modeling because of poor visibility in the feature tree.
Someone digs this up about every other year. This doc was produced using UG, but I have seen the technique mostly used by Pro/E users. You know when you import a Pro/E native file, you get a bunch of planes? I think Pro/E must teach this method. It is an extremely conservative way of working, very slow and it seems like you do all of your work twice and have to think about it hard before you actually do anything. The big benefit comes when you start making changes. Face and edge ids depend on intersections, and when the intersections change, so do the ids. This makes it difficult for models to cope with big changes.
What this article is calling "horizontal" modeling is just a set of best practice rules for creating relationships in parts and assemblies. Essentially, you work by first creating one or two or three sketches on the XYZ planes that locate the major features of the part, and where ever you need a sketch, you make a plane. So you never sketch on a face or reference an edge or model vertex. In SolidWorks there are limitations to how far you can go with this technique. You have to select model entities to create fillets, chamfers and other features, and it is really only well suited to prismatic parts, because in more shapely parts you have to reference faces to match curvature, and edges can only be defined by face intersections, not by an independent layout sketch.
I use portions of the method, primarily layout sketches. Recent versions of SolidWorks make it easier to reuse sketches, and use only portions of sketches, which help a lot. But with surface modeling, you are building from existing edges, and it is difficult to reconcile the methods. I submitted an abstract to present at SWWorld this year on "SolidWorks Relationship Counseling", where I plan on talking about the method of using layout sketches and planes, and always making relationships to things as high up the tree as possible. You can use the concept in parts and assemblies. This is essentially the same as what is being discussed in the article and the pdf.
SolidWorks, when it was introduced in 1995, focussed on "ease of use" in comparison to Pro/E and UG, so they didn't worry so much about best practice. Best practice is conservative, it is slow up front but if it saves you time it will be on the changes. SolidWorks wanted to be quick and easy, so they advocated a very "fast and loose" method of working from model faces instead of planes and using model edges instead of layout sketches. I don't think SW corporate has ever out grown this "fast and loose" attitude. This is why users are so surprised when they come across stuff like "horizontal modeling".
It is essentially removing the dependency on "history" from the model as there is very little. Most features planes and sketches are constrained to default origin planes/coordinates. Makes for little if no design intent though.
The first time I tried to defeature a Pro/E model I found out about just how hard not using horizontal modeling can make things. Although Pro/E had some neat features for reordering the interface was very difficult to use because every feature had a number, not a name. You had to know what feature the numbers referred to. That is one reason I fell in love with SW way back when. But times have changed and the complexity of the models I make has increased. Now many people push SW and in this area it needs a facelift.
jb (below) actually makes some good points, implications. Many good software companies, almost by dint of being good, went belly up. It seems going bankrupt/removal from NYSE does not reflect a bad company/bad product, but a corporate structure short on MFQ--MuthaFucka Quotient, and thus unable to survive among other entities with much higher MFQs.
The Consumer, in their infinitiesimal wisdom, create and perpetuate this scenario: Fuck me, and I'll reward you, it seems.
It's weird, but I learned a lot about solidworks from using xsi. The difference is I think the documentation on each software is geared towards a different modeling approach for different modeling applications. All I can say is thank you shareaza.
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