Can any one help me on the following.
I have an assembly made in ProE 2001. Can I just make changes to the assembly alone ? I do not want any change to its associated part files and drawing files.
Is there any special method to do this ?
There are several ways of going about this:
- The first is to make the changes in the assembly; any features created using Feature | Create in assembly mode will be created as assembly features. These are not specific to a single part, but rather, are contained in the assembly. Typically these are used for things like a cut through multiple parts at once (in real life, you assemble it, then cut it). Since you don’t seem to want to change the parts themselves, this sounds like what you need. I’ll include the other options, just so you know what else can be done.
- Another option is to make your changes in part mode, and then see how they turn out in the assembly. This is preferred if you don’t want to create dependencies on the assembly file, and/or other parts. Perhaps the part is used in a different assembly, which you don’t want to reference.
- The last way is to use (on the right-click context menu) Insert Feature. This will allow you to create a feature that is stored in the part file, but which can reference the assembly. It creates lots of dependencies, though, so you need to be careful using it. (I use it a lot for gearboxes.)
Thanks yar.
I am now confident I go ahead. Thanks a lot. May come back for future probs !!!
Let me get this out of my system.
DO NOT USE ASSEMBLY CUTS OR FEATURES IN PRO/E
They cause all sorts of reference issues and if you select the wrong options when creating them you can cause all sorts of problems. This is more of an issue when multiple people are working on an assembly but the consequences are sitll the same. This is the easiest way to cause a cicular reference and should only be done as a last resort.
Now that I’ve had my soap box speech what type of feature you want to create really drive how you should do this. Make sure to not check the modify part option when when making an assy cut if you don’t want it to effect individual parts, this is where the the references that cause issues get created. The reason I suggest not doing this is from personal past history of large assemblies crashing from circular refs. The problem is not the commands but the inability of most people to use them properly. If you are are careful and read all the prompts you won’t have any probelms. I still however never let designers or other engineers working on my program do this.
Pete
This is where design intent, manufacturing intent and program functionality clash. If the intent is for a cut to be made through the assembly, and not individually on each part, the assembly cut seems logical–but for the reasons you describe, things can get a little crazy when chasing the references later on, because of Pro/E’s need to maintain dependencies. (Note that for the same manufacturing intent reasons, assembly protrusions don’t make much sense at all, in most cases.)
If you’re going to be putting the parts in other assemblies, definitely treat it like the second case, or the third case (if you’re very careful about what assemblies it will belong to). If you’re going to leave it all in one assembly, occasional use of the assembly cut should be fine–but it isn’t intended to replace individual part features. I would avoid other sorts of assembly features, if they aren’t sensibly grounded in either design or manufacturing intent.
Most importantly, whichever technique is used, good practices should always be followed when choosing references: don’t pick features that are prone to disappearing or changing, as the model evolves; try to use as few references as possible to constrain the sketch; avoid references on separate models in an assembly, if a single model will do (mostly for Insert Feature).
In short, “never” is probably too strong, but if in doubt, you can still take the safer route, and modify the underlying model. With a little experience in choosing references, you shouldn’t have too much trouble making a good decision.
I know it’s strong but, and this specifically for business purposes not FIRST, I find it makes people think much more about how they will make the part (in Pro/E and reality). This frequently works to eliminate these types of design choices. I don’t like to let people get away with doing what is easier for them in a CPU rather than what works better on the assembly floor. These problems get magnified when you start using PDM, PRO/Intralink, or PDM/Link a a data vault. The fear is a change on a part has impacts down the line that someone is not fully aware of because they are only working on an individual part not the whole assembly. The impacts can become a configuration control nightmare.
My feeling is that if do not have an appreciation for the full implications of assembly cuts or features you should not use the function because of PRO/E’s inherent parametric referencing. These problems all get magnified when you have multiple users working on assemblies and subassemblies who don’t know how all the parts were modeled.
To sum up if you have multiple people using your models are don’t realize the full extent of PRO/E’s parametric referencing using this feature is a bad idea. If you’re just trying to do a quick and dirty FIRST drawing with no configuration control it probably won hurt you.
Pete