View Single Post
  #16  
Old 05-22-2007, 02:57 PM
Steve Steve is offline
Registered User
 
Join Date: Mar 2003
Location: Alabama
Posts: 309
Re: OneSpace vs. SolidWorks

Marten:

Quote:
With history based modeling you have to think hard all the time, when you are creating a model. You have to think: how would this model be changed in the future, because if you don't build the model in an appropriate way, it will be harder to modify. This won't be a big problem for easy parts, but it will be a big problem with complex machines.[
Actually, your thought process should be like that of anyone who is considering the fit, form, and function of a part they are designing: "What relationships are important about this particular geometric feature?

Yes, this takes careful thought with the creation of each feature - as it should if you are a careful engineer. Not a single face exists on a part without a purpose, or you would not have put it on there. Why not capture what that purpose was?

Quote:
For example: you model a flat metal part of 500 mm long. Then you add 5 holes evenly divided, in a linear direction. Which design rules do you add here? Is the line of holes always centered to the model, or is it always on the same distance to one side? How many holes are needed? When I make the part 1000 mm long, do I still need 5 holes, or do I need more? When you are creating the part, you can't answer these questions, because you don't know how the part will change in the future.
It isn't so important how the part will change in the future, but rather, what is the current design intent.

If your design intent is to have 5 holes evenly divided along the length of the part, you parametrically establish that sort of pattern so that no matter how the part length changes, you will always have 5 holes evenly divded in that linear direction.

If your design intent is that the holes need to be centered to the model, then you establish that relationship.

If your design intent is that the holes need to be on the same distance to one side, then you establish that relationship.

If you don't know how many holes are needed if the part grows in length, then you have an engineering problem, not a CAD problem. Once you have determined the engineering requirement, then you can set up your model so that when the part is, say, less than 1000mm long you have 5 holes, and if it is over 1000mm you get 6. Or you can even set up a relationship to drive the hole array to achieve a certain "negative area" - the amount of open area the holes are required to provide based on the number of holes present and their size.

If you can't answer these questions at any particular time in the design - NO PROBLEM - you don't HAVE TO. Many parametric, history-based software packages such as Solid Edge, Solid Works, and others don't require the constraining of sketch geometry in any way. The point here is not that you have to create design relationships in your geometry, the point is that you can. I tend to lock things down just as soon as I am able. Why? Because I can forget about them from then on and they will take care of themselves.

Quote:
How these holes are positioned, and how many you need depend on how you are going to modify it.
Absolutely, 100% incorrect. How these holes are positioned, and how many you need depends on engineering requirements, and is completely unrelated to the CAD software. The point here is that once you have defined the engineering requirements, parametric software allows you to capture those requirements.

Quote:
Where is your 'advantage' of the history in the model? It did take more time to add the rules, and now you even have to dig into the models history to find out how you can modify to get what you want.
Well, the way I see it, it's the "pay me once now or pay me forever" problem. You can either take the time to codify the engineering requirements once such that the geometry flexes while obeying those requirements, or you, and every future designer can manually maintain those relationships with every model change forevermore.

Quote:
But you aren't finished yet. After you have modified the model, you have to check if other parts didn't modify in an unexpected way. The part that is bolted to this model, did it stretch when you stretched the model, or did it move, or didn't it get changed in any way while it should?
Certainly it is true that if the engineering requirements were not correctly codified in the model it will not flex properly automatically. Of course it is also true that without the ability to capture engineering requirements at all your model will never flex properly automatically.

Quote:
All this burden is even more restricting when you are designing completely new machines, where you don't exactly know how it will look and function. You will likely change a lot during the design process, and you constantly need to think about the design-rules, even if you don't know (yet) what they are. And because it is a history based modeler, you have to invest the time.
As I said above, many parametric modelers today do not require creating design rules. In this regard they will function much like CoCreate - you just leave off the parameters. Yes, the history aspect of the model means that some features may be dependent on previous features and this can be annoying during editing of the model. The good news is you can generally re-order features fairly easily.

Quote:
Now another example. You created an assembly a while ago, and now need to create something similar, but nonetheless different. If you use this model in a history based system, you also 'inherit' the design-rules a.k.a. history. For this new assembly, these design-rules probably don't apply, but you still have to study them and modify them in order to modify to model the way you like.
Yes, this is true, and logical. If new design requirements are in play, then the geometry will need to be modified to obey the new requirements.

Quote:
n your post, you have the example of the cylinder where a taper is applied to. In order to modify the diameter in the history-based system, you have to know how the model was created, or you have to study the history to find out. Is the conical face created by a taper, or is it created by revolving a cross-section?
No you don't. You just double click on the geometry right on the screen, and the appropriate dimensions light up right there for you to edit. You can instantly see whether you are dealing with a taper or a revolved section, and, either way, directly edit the taper angle or the underlying untapered feature.

Quote:
In OneSpaceDesigner you need a few commands to do this. The offset-command can be enhanced in order to make this easier, but you definitely don't need to do trigonometry accomplish it. (You can un-taper, change diameter, re-taper or you can draw the new diameter on a workplane and offset the face while using measure to determine the distance.) It's not as hard as you pretend.
It is exactly as hard as I "pretend". If you want to change the basic diameter of a tapered cylinder in CoCreate you have two options: Untaper the cylinder, change the cylinder diameter, and then taper it back, or do trigonometry to determine the normal offset. Drawing a circle on a workplane normal to the cylinder axis will not help you because measuring the distance from the conical base to the circle will not give you the normal offset required to hit that circle. Deleting the taper (untapering the cylinder) and reapplying it is not as efficient as simply directly editing the underlying basic diameter, not to mention all the drafting havoc you create for dimensions and such that were tied to the taper.

And the heck of it is, this is a trivial example of the problem. Try modeling up injection-molded or cast parts of any complexity at all and then have a need to go back and modify the underlying basic cavity sizes that have all been lost under drafts and blends and you will find yourself pulling your hair out. I know from experience.

Quote:
A history-based system tells you precisely what feature is failing down the history-path. The versions of SolidWorks I used didn't tell you why that particular feature failed either.
I've never used SolidWorks, so I can't speak to it. But in both Pro/Engineer and Solid Edge, when a feature fails, it usually provides some diagnostic information as to what is causing it to fail. At the very least, though, even if you want to follow the hack-and-slash method of deleting problem features rather than fixing them, like you have to do in OneSpace Designer, at least you know which features to delete.

(continued)
Reply With Quote