When i use copy geometry, i get 3 different choices for updating the feature when regenerating. Automatic, manual or to just make the copy independent.
If i set it to be "indepentent", the coped geometry will offcourse not update, and you can´t see the connection using reference viewer or in PDM link. ( thats seems logic to me) . The connection is still there since you can set it to automatic again, but creo will not show it.
If i set it to be "manual" , the copied geometry will not update since it´s supposed to be done manual. If i go for "edit definition" on the copy feature , change nothing and then click ok, the geometry will not update either. If i regenerate i will not update. So to make it update, i have to set the feature to be automatic and then regenerate, and then put it back to manual (if thats what i want) . The nice thing about "manual" is that i can still see the connection in ref viewer , but i have control of when the geometry should update.
So, my 2 questions are :
* Is there some other way to just update a "manual set copy geomerty" than to put it in "automatic"?
* Whats would you say is the benefit of having it in manual and not independent , more that you can find the connection in PDM link and REF viewer?
Hi, I am assuming you are using Creo 3?
There are no such options in Creo 2 and i would like to find out from you (instead of answering your questions, ) what would these options do for an external copy geometry feature:
If I need to move the location of the copied references. Do I need to bring the parent model in session ?
Correct, i´m on creo 3.0
Well, if you want to update your geometry in a children part, your parent must always be in session. Otherwise i assume that the children doesnt know something has changed in the parent part.
The parent will automatically be added to your workspace (if you use pdmlink, cant remember how intralink works...) if you "edit definition" your copy geom feature. If the parent is not in session ,then i suppose it doesn't matter if you have it set to any of the 3 options I asked about, the children will not feel any need to be updated at all 🙂
Or did i misunderstand your question?
In our case, we always copy geometry and place it using coordinate systems.
My question is if there is NO change in parent geometry, but i merely need it to relocate in my model by adjusting locating coordinate system in my model. In this case, do you still need to bring in the parent model into the session?
If the update control is set to "automatic update", then as soon as you do a edit on the c-sys, the parent jumps in to the session. ( as you said, no change in the parent geometry) .
If you set the control to be "manual update", then you can edit your c-sys placement and relocate your external copy geometry around as you like, without having the parent automatically added in session.
the new function "Independent" is loosing the references to original part. Even PDM will not create a ghostpart anymore. I just made a test. So be carefull this is a oneway decision!
To avoid data retrieval, you can "set retrieve_data_sharing_ref_parts" to no. This will not add the referencepart in session. The Default value is "no".
This can cause data wich is not uptodate. The benefit is faster retrival.
So finally I would say the "Independent" button is new and the option for Information.
Well, actually the "independent" is not a new function. The option has been there before. What changed , and i believe this is a datecode change? ( as we tried the function 2 weeks ago, then updated to a new datecode last week and we got a different result today) is like you say " Its a one way decision". In previous releases (and the datecode we had before , still using creo 3) you could turn off the dependency and then turn it back on again. The result when it was turned off was that you couldn´t see any connections in PDM link , but you still had the option to turn it back on in creo and everyting is back to normal again...
As for now, if you set it to independent, like you said you can´t turn the dependency back on. (or is there a config for this?)
In this thread below , Doug wrote: "Setting the copy geom to independent does not remove the reference to the original part, it simply means changes to the source will not propagate to the target. They are still 'tied' together and you can later set it back to dependant if you'd like."
So, since the function has changed in the latest datecode of creo 3.0 , that means "indepentent is a one way decision", the answer to my second question is pretty obvious.
But i would still like to know, * Is there some other way to just update a "manual set copy geomerty" than to put it in "automatic"?
I'm replying to this relatively old thread hoping it gets bumped and noticed.
Does anyone know of a solution for updating the data sharing features that have been set to "manual update" other than turning them to be "automatic", regenerating and then turning it back to "manual" (and regenerating)?
It's rather annoying especially if you are dealing a model that takes half a day to regenerate...
For copy geom features, then the right-click menu provides a convenient shortcut to toggle the automatic / manual update and you only really need to do the regeneration once.
However, if you need to update a merge feature, this takes 2 edit-definition steps and hence 2 regenerations...
I would add only one thing:
Copy Geometry: If the customer has Design Exploration (DEX) license, then has option Update on Right Mouse Button.
Shrinkrwrap feature and Merge/Inheritance: No option Update on Right Mouse button.
As written in previous post, for Shrinkwrap and Merge you have to Edit def > Automatic > Regen > Edit def > Manual > Regen.
Thanks for replying. So it is as I suspected. It's nice that the new features (DEX) have user experience enhancements, but I wish PTC would go back and improve the old features as well. I'll see if I can raise a product improvement idea (I don't have a maintenance account).
Well, I can't make an idea, but there is already at least one in place about this issue:
Vote early, vote often!