Is it possible to pick features and dimensions in assembly mode?

Greetings:
I have 4 components assemble together. I would like to make a family table in the assembly mode. However, when I click on individual
component or the entire assembly, there aren't any dimensions or features that I can chose from. Is it possible to make the components features along with its dimensions available in the assembly model tree?
Thank you in advance for your time and help.
John
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I've never done it, but believe what I'd try to do is make Family Table instances at the part level, then look at replacing part instances in each assembly table instance. (? Sorry, haven't got time to try it out right now, so apologies if I'm just blowing smoke.) Another possibility might be Flexible components. What version of Pro/E? Might be pertinent?
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... and last, but not least; maybe just drive the part features you want to change from the assembly.
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: Greetings: : : I have 4 components assemble together. I would like to make a family : table in the assembly mode. However, when I click on individual : component or the entire assembly, there aren't any dimensions or : features that I can chose from. Is it possible to make the components : features along with its dimensions available in the assembly model : tree? : The tough thing to figure out in trying to make a family table from an assembly is what can you do at that assembly level. And that's a very good question ~ what can you do at the assembly level. Well, you can include (assemble) or exclude (suppress) components. In a family table of an assembly, the Component selection is asking you just that: should this component be included. Suppress the component and pick 'no' to include it (yeah, I know, this is a cheap trick, double negative to make a positive, but what's the alternative? you can't cancel an assembly of excluded, cancelled components. Pro/e doesn't work that way!!); assemblies let you adjust dimension values of component offsets; assemblies let you create and modify assembly features, selectable as features (yes/no) in Family Tables and it will also let you pick some dimensions of these assembly features as 'Dimension' ( but you can't select part features for a family table at assembly level because they aren't accessible/controllable at assembly level.
So, in summary, at assembly level, you can control inclusion/exclusion of components (by suppressing at assembly level then selecting NOT to suppress); similarly, inclusion/exclusion of assembly features (suppress at assembly level, elect not to suppress in family table to include); dimensions of assembly features or assembly 'offset' mates/aligns; feature also is yes/no so you must start with a feature suppress to include it. The whole thing comes down to looking at what can you do at the assembly level. There's a smalll trick at assembly level (activating parts, modifying parts or creating part features, using the other components in the assembly as reference), but this does not make it into family tables. I may be mistaken, but I do not believe you have control over part features at the assembly level in Family Tables.
David Janes
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Thank you all for your insight thoughts and help.
I hope that there is a way in WF2 that would allow me to pick up features and dimensions create in part mode like Solidworks does. I think this will save users a lot of time and typo. Effectively, if my assembly has more than 30 options (each component has an average of 5~6 instances). It would be a real pain to manually type each component instance name, click "yes" or "no" at each cell. Don't you think? Is there at least an easy way to avoid typing all the components instance name? If not, I think SW is really shine in this particular situation.
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In part mode or pick part features and dimensions in assembly mode? Former is possible, latter isn't, in WF2, to the best of my knowledge.

Not sure if I understand. When you create a new family table instance row all the column values default (denoted by an asterisk) to the generic. You only have to enter values for the changes.

See *** below.

Don't know how SW does it. It might. Could also be that Pro/E's stricter structure makes it a more reliable or easier to resolve problems or failures, maybe even quicker to regen?
I'm not sure if this corresponds to what you want to do, but.... Let's say I have a strut assembly; tube, clevis yokes, taper pin connections, holes are assembly features. I want to make a bigger version with an additional taper pin in each clevis attachment. One way I might go about it is to (I'm making this up, learning it, as I go. It might not be the most efficient or versatile way. Might not even the "right" way and hope someone will correct me if I'm screwing up) ....
_ Open or activate each part that will be modified and create a family table instance. _ Create a family table instance of the assembly. _ Create columns for the components that will be swapped out. _ Type in the instance name (replacing the Y / N / *) for each replaced component -OR- *** Tools / Replace Using / Famly Member. Also look at the Assembly Instance Configurator (Tools menu) _ Open the new assy instance. _ Add the new holes (assy features). _ Add the new pins. (The new features and components are added, suppressed, to the generic and the family table.) _ Close the assy instance (back to the family table dialog in the generic). _ Verify the instance generation and you're done.
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Jeff, thank you for your detail explanation.
Let assume that I have 4 parts with 4 instances in each part.
A-1, A-2...A-4 B-1, B-2...B-4 . . D-1, D-2...D-4
I assemble these 4 parts together using the generic, then create an assembly family table for each of the above components. In order to show all the combination of each part instances, I need to type in manually each instance name A-1, A-2,...,A-4, B-1,....D-4 for each cell. It would be easy and simple if the instance name has just a few character long; however, it would be a great pain if the instance name have many character such as P/N.
In SW, once you assemble each components together. The components show in the assembly's model tree along with its features. If you want to create a family table, you just need to double click on the features, dimensions from the part level right in assemlby mode and they will automatically appear on the cell. No need to type in all the lengthy P/N instances.
If you don't see any incovenient, I can send you the assembly file in WF2 so you can have a better picture of my explanation.
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No prob. Trying to figure out what it's all about as I went.

Sounds interesting. Don't know any way to lighten the load except maybe to edit in Excel where it's quicker. (Let's see; 4 ^4 is 256; still a lot of typing.<g>)
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: Thank you all for your insight thoughts and help. : : I hope that there is a way in WF2 that would allow me to pick up : features and dimensions create in part mode like Solidworks does.
I see, you were hoping that Pro/e was just the grown up version of SW and that you wouldn't actually have to learn a new program. Sorry to disappoint. It's been around a bit longer than SW which hasn't even been taken seriously for mechanical design until the last 3-4 years. So, we have separate evolutions going on where Pro/e provided the standard in advanced functionality and SW has been giving some basics at a drastically reduced price while playing catchup on the advanced stuff. Moreover, PE has been well established, for over half of its 20 year history, on the Unix platform, coming to Windows only after NT got established, about the time that SW got its start. Now, with respect to developing a GUI interface and making modelling functionality more user friendly, PE is making a good effort but is the one playing catchup. None of this history should lead anyone to expect that PE and SW would work the same. Rather than comparing based on certain prejudices, the best thing to do will be to get to know how PE works, how a very complicated functionality like family tables works, before trying to make comparisons or recommendations.
One reason for saying this is that you are somewhat confused about how PE works. In your post of 10/20/04, you said the following: "I assemble these 4 parts together using the generic, then create an assembly family table for each of the above components." Well, no John, you don't. The generic, once you have a family table of part instances, is invisible. You assemble instances, already named in the table. These instance names are effectively file names and may be treated as such by Intralink or another PE compatible PDM/PLM system. Also, while your assembly is composed of family table instances, it is, itself, not part of a family of assemblies. That happens only when you go to 'Tools>Family Table' and create a table of your assembly where certain parts vary. They can vary by being there or not (suppress a component or not ~ yes/no parameter). Or, if you use 'Edit>Replace>By table' to pick another instance of the same component from the table, this will be incluced in the table as a new instance name. In fact, in your assembly table, your next assembly instance can have all new parts. It requires onlyh that you go into the assembly and do an 'Edit>Replace' on a selected component and replace the component with another instance from the table. You don't mess around changing sizes in the assembly; you change assembly components, swapping out one for its leaner cousin, a couple cm. smaller and thinner.
There's a lot to it. It can get quite complex, but, as I said before: learn how PE works before you start comparing.
: I think this will save users a lot of time and typo. Effectively, if my : assembly has more than 30 options (each component has an average of : 5~6 instances). It would be a real pain to manually type each : component instance name, click "yes" or "no" at each cell. Don't you : think? Is there at least an easy way to avoid typing all the : components instance name?
Yes, you can avoid typing instance names when creating a family of parts by using the Pro/e 'patternize' function. With the generic part open, go to 'Tools>Family table>Edit', pick a dimension, parameter, etc. to vary and add it to the list of variable elements, set the number of times to repeat and the increment value. When you press 'ok', it creates, for you, as many instances as you indicated, giving them all an icremented instance name: no typing necessary. In fact, there's very little typing at all in PE. Just as in SW, you pick a dimension to add it to a table; if you select parameters to vary or patternize, PE gives you a list of parameters available so you can pick from a list (again, no typing).
However, you've said some things, supposedly bragging about how much easier SW is than PE, but they don't stike me that way. I took a course in SW, recently, did some configuration stuff, enough to roughly compare with PE and wound up with the impression you created, talking about your 30 easy configurations. Well, the impression was more some questions. Like, don't you have to spend a good bit of time naming these 30 configurations, trying to keep them straight, trying to distinguish one from the other? In the Configuration Manager, you type in these names, don't you? And, because no name is really sufficient to distinguish, you spend some time filling in discriptions? Doesn't seem you're getting away from typing. But the main thing I wondered and never got settled (maybe it was the junky book we used, not much good training material on SW, even SWC doesn't provide any) was this: how do you convey this information to production? How does the program keep track of how each part/component is varied? How do you know if you're repeating yourself, i.e, does this configuration already exist? Does this configuration business result in families of parts? Can you get documentation of this series of parts (and what varies) by easily producing a series of drawings based on this part family (again, something that production absolutely needs)? Can you order any of the parts in your assembly configurations without part names/part numbers/descriptions/vendor information/etc and, if not, how do you get away without typing it into parameter fields? Well, they did it without significant typing, at one place I worked, by harvesting the numbers and making tables from the data of an MRP system. This was how they went from 2D to 3D and got into PE family tables with thousands of instances in dozens of tables and fifty fields per table and almost NO TYPING!!! Is that how SW works, does it encourage this kind of design automation or does it simply give you the illusion of doing stuff quicker.... manually!?! Really, learn how PE works and then try to compare.
David Janes
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David,
Thank you for taking your time on this. Admit that without the comparison between SW and WF you wouldn't give out these little xtra secrets, wouldn't you? Just joking :-). Anyway, your comments and insight thought is greatly appreciated. I will take a harder look at these new (it's totally new for me) additional technics in Pro/E.
Also, I just want to point out that my comparison has nothing to do with competition between two Mcad package or to promote either software but rather to seek and learn a comparable & efficient way to perform the same tasks between these two when ever possible. I understand each one has its own strengths and weaknesses and a perfect MCAD simply doesn't exist.
Happy Pro/Engineering.
John
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