an issue with part flexibility

[xureta]

I am using Creo Parametric Release 4.0 and DatecodeM130

I have a part with flexibility (adding and suppressing some features). I want to create a drawing of the part with the different flexibility status. How can i do it? How can I represent the different flexibility status on the part (not on an assembly)?
Thanks

[tbraxton]

A family table with an instance for each configuration would handle this within the part model.

https://support.ptc.com/help/creo/creo_pma/usascii/index.html#page/fundamentals/fundamentals/fund_ten_sub/About_Family_Tables_1.html 

Your use of the word flexibility in this context may be misleading to other users. Flexibility has a specific meaning for Creo Parametric functionality, and I do not think it applies to your situation based on your description. Flexible components are the area where the term is used.

[StephenW]

Flexibility, in terms of intended functionality, is supposed to be an item like a spring or o-ring that is in one shape or form with in a free state but takes another shape or form when in an assembled state. It can only have that "alternate" shape when assembled.

I do understand (or I have done/seen/used/drawn) something very similar to what you are asking. A spring drawing showing a free state, a compressed state/ stretched state. Usually along with some values of what the expectations are for those states. I have in the past simply used sketched curves in the model to show those.

[Dale_Rosema]

Similar to the other responses, I have made family tables (create separate instances) where the assembly "uses different" parts, which are the same part but modeled in a different state - extended or compressed. Then I just use the two instances of the same part as needed in the drawing to show the two "states" of the assembly.

[Patriot_1776]

If you're "adding and subtracting" features, that's a Family Table part and you're swapping out instances.  As mentioned below, there is actual "Flexibility" which, as mentioned above, can do things like give you compressed springs, o-rings, but also fill out your BOM differently.  For instance, my fasteners can be used where you can enter a mil-spec and mil part number, or you can use a vendor name (i.e. McMaster-Carr) and part number, and depending on what you enter it will fill out the BOM however you want, and you can change the material and finish however you want as well.  Or you can not use those parameters at all and you'll simply get the standard description (i.e. .250-20 UNC-2A X 1.500 LONG) in the BOM, useful for companies where you simply grab fasteners from a bin in the back and don't need mil-spec or vendor part numbers.

For what Dale mentioned you can create different "Simplified Reps" so that you don't get 2 different springs (if your assembly has different compressed heights) in the same BOM, but make sure the rep you want the BOM to represent is the current rep BEFORE you add the BOM table.  Repeat Region BOM tables take the parts in the current "Rep" to populate the table.  It's a little trickier than all that, but that's the gist of it.

[xureta]

Hello,

Thanks to all of you for your answers. In my company we haven´t got goof experience with Family tables in Windchill, therefore we prefer to avoid this solution. In the case of simplified representations, I have to create different shapes for different stages of the part, the problem is that for the weight calculation, Creo is taking into account the geometry of the different stages (Master representation). Is there any way to avoid it? Could we take into account the weight of a certain representation?

[tbraxton]

Assign the mass properties as required.

https://www.ptc.com/en/support/article/CS60265 

[xureta]

Thanks for your answer, but I don´t want to assign a certain weight value, I want Creo to measure the part at certain stage of flexibility (or if it is necessary at each simplified representation)

[tbraxton]

You would be better served by responses if you were to more completely detail the problem statement and all of the conditions imposed on the solution space. If the mass of the part is changing, that does not seem to be a flexible component function application unless I am missing something. Elaborating on the nature of the part and the "flexibility" would help.

If the mass of the part is changing that would suggest you are adding or removing material to the part.

[xureta]

At the end I need the part when it is assembled is deformed at different stages, so that the mass does not change. But if I need to create the different geometries that shows the evolution of the part,  the weight is taking into account all of them. I would like to get the weight of one of the stages (the same for all the stages) as it does when it is assembled.

[tbraxton]

You can use simplified representations in the assembly to exclude components from mass property calculations. You would then be able to obtain accurate mass props for each state of deformation of the "flexible" component. You can also filter drawing view visibility using the simplified reps. 

[Patriot_1776]

So, this is some stamped sheet metal part then?  Well, if you're seeing a variation in weight at the different stages between the ACTUAL part and the part as modeled, then obviously your model is wrong and does not reflect accurately what the process is doing to the part at each stage.  Now, that's easily done because to my knowledge Creo cannot actually create the geometry that actual sheet metal processes produce, such as localized stretching (and thus thinning) or the material in areas.  It just assumes a constant wall thickness no matter what the forming operation.  So, if you expect that Creo will give accurate weights for that kind of thing, it's not going to happen.  As Mr. Braxton mentioned above, you'll need to assign weight based on parts actually weighed.  I've never had to add that info at the family table level, but I would think that parameter could be added to the table.  It's been forever since I had to assign a mass/weight to anything.

[BenLoosli]

Family tables are not an issue in Windchill as long as you have control over them. 

I have over 30 family tables with over 11K parts in them in Windchill. These are mostly COTS hardware items.

I have done assembly family tables in Windchill and they worked okay, but then I controlled them and was the only one adding new instances.

[Patriot_1776]

EXACTLY!  Some of the people I work with have ZERO clue about how to use family tables, and instead would rather download GARBAGE fasteners from McMaster-Carr (or similar) rather than use the extensive fastener tables I've created that actually work with the repeat region BOM tables I've created.  I found the best thing to do is add the generic to your Workspace, and immediately LOCK it.  That seems to prevent the entire table from magically appearing in your Workspace, which was one of the gripes the ignorant had about using family tables.  They just accidently checked out everything to their Workspace initially or did when it prompted them.

When we were still using the SUPERIOR PDMLink, there was a way I could "Lock" the files at the vault level to prevent this, but in Windchill I haven't had any luck being able to do the same, so my advice to anyone using them is to Lock the generic immediately.

[BenLoosli]

There is a setting that will make library files read-only when downloaded to a workspace. I have it set in my Windchill.

[Patriot_1776]

'Morning Ben!

Do you remember the setting?  Is it a Windchill setting buried somewhere?  The problem right now is that I'm not the "Owner" of the folder the files are in so I have no ability to set certain settings, I'm trying to get them moved into the folder I AM the owner of.

Thx!

[BenLoosli]

Found it by search the knowledge base!

PTC Windchill Help Center

You can set the Automatically lock objects added to workspace preference to Yes to lock all objects, by default, as they are added to the Workspace. To lock only objects you do not have Modify access for, you can set the preference workspace.autolock.for.no.modify.permission=yes in the wgmclient.ini file

[Patriot_1776]

Ah, thanks!

Unfortunately, I want to lock this at the Comonspace level like I used to do with PDMLink, since I can't trust all the different users to set their local preferences to do this and I don't have the permissions to make global settings changes.  Drat!

I guess what I COULD do is just keep everything checked out 24/7 to a local Workspace and that would do it, but then that means I have a huge local Workspace filled with parts, just so I can "Lock" them.

Thanks for the info!

The search continues.