Need to be able to change the parameters from the skeleton model but from within the machined file.

[ER_9260823]

Hi,

I know this post is old but want to understand what did it end up going with?

I have 3 files.  

The first is a skeleton with the dims i need to drive

The next model is the cast version

last is the machined version.

I need to be able to change the parameters from the skeleton model but from within the machined file.

TIA

[tbraxton]

You should open a new thread for this. Define the parent child relationships between the 3 models you mentioned. This will determine what options are available to you.

Are you using an inheritance feature to create the as machined model from the as cast? If not, how is it set up? The mention of a skeleton model implies that you are controlling some design intent in assembly mode, so you will need to define how this is set up as well.

Is your design intent structured such that the skeleton model is a child of the as machined model? This would be unusual for Creo parametric as the top-down design paradigm would suggest that the skeleton model is a top-level object used to distribute design intent to multiple children.

[ER_9260823]

Thank you.

The skelaton model publishes geometry at the end to the CORE and the CASTING

the Casting, core and machined part all nearly start with Extern Copy Geom Id...the Casting and Core reference the skelaton and the Machined references the casting.

If i put them in 1 assembly i see all the parameters...but i want to be able to if i only load the machined model (but have the other 3 files in a searchable directory

TIA

[tbraxton]

I have created an intent map based on your written description. Confirm that this is accurate.

Your skeleton model is a parent to the core, cast, and machined part models.

Your objective is to open the machined model only and modify the model parameters of the skeleton without having any other models in session. This is not possible with the structure in the above map. 

If you want to control parameters that are shared across multiple models from a single file, a notebook (.lay) file is the best way to handle this. The notebook would define the parameters and then you declare the notebook to any model that needs to use the parameters. This enables the use of global variables (parameters) across the design space.

https://support.ptc.com/help/creo/creo_pma/r9.0/usascii/assembly/asm/About_Notebooks.html 

I should also mention inheritance models as they were specifically designed to deal with the design of cast parts in Creo. Using inheritance features you create a master model for the raw casting and then use this to drive a derivative (child) model of the as machined version of the part.

https://support.ptc.com/help/creo/creo_pma/r9.0/usascii/index.html#page/assembly/asm/To_Create_an_Inheritance_Feature.html 

[ER_9260823]

Thank you very much!  

I believe that is an accurate diagram.. 

That makes sense about not having them in session,

I had thought If all 4 files are in the same folder, and i open the Machined, it would require the 3 other files to load into session, But that does not seem to be the case...It must load the geometry of the last saved version and not run through the tree?

Is there any way to force the other 3 files to come into session when i open the machined file?

WRT notebook ...It sounds like i would go in and update the skeleton and the machined would get updated?  Vs being able to update the skelaton dims from within the machined model?  That seems similar to what i have setup where the skeleton is essentially the notebook because if i go in and change it, the machined model will update

WRT inheritance, the help seems to indicate its for passing parameters between parts in an assembly... can't tell if it would work if the parts are not in an assembly like i have.

Temporary work around is if i make a new assembly and put all 4 files in, if i update the skeleton, all 4 update including the machine model, then i can export and delete the other 3 when i import them into my sim tool.

If there is a way to be able to load the machined model and it loads the others into session or provides the workflow needed, I'd be happy to revisit the setup.

Thank you very much!

[tbraxton]

It seems you are attempting to do something that would create circular references if it were even possible. The machined part is at the lowest level if dependency, it should not be controlling any if the parent objects above it as shown in the map. I may be wrong about this if I am misinterpreting your stated goal. Can you elaborate on a single example of a parameter in the context of this design, it may help clarify things.

Terminology is critical here. When you write "parameter" it has a very specific meaning in this context. I suspect you may be referring to dimensions and not parameters, so please confirm.

In order to have Creo attempt to retrieve all parent objects I would need details on dependencies. I do not think this is an objective that you should try to manage. Creo only retrieves what is needed by design (to minimize loading to RAM/in session objects).

Without access to the models, I am not able to comment on automatic retrieval when opening only one model. The copy geoms do not regen on model retrieval so I would not expect Creo to search for the parent model of the ECG features. If the ECG is the only external ref to a parent model Creo would not retrieve it when opening the machined model.

Notebooks are always at the top level of the design structure. You would define the relations and parameters to be shared across the models in the notebook and then declare the notebook to any model that needed access to those definitions. This means that you could manage the parameters and relations from the notebook and drive all of the parts from this single file. A notebook does not contain parametric geometry. Think of it as a "folder/model" that is a container to define global variables and relations for use in dependent Creo models.

I will try to dig up more info in inheritance features used for casting design. Your assessment is far from complete in terms of functionality.

Focus on defining design intent and then capturing design intent with Creo functions. I have designed castings (sand, investment, die) that have required post machining etc. and the preferred method is to use merge/inheritance to manage it as a top-down design. There are other ways to manage it if the design intent/workflow warrant it but I need to know details to comment on the best approach.