I am Creating assembly Drawing. Usually we create REP to for View clarity for views other than main view . But Now i am unable to use parametric balloons on views with different REP. any way to fix this. BOM balloons is from Master REP.
Unfortunately it is not currently possible. There is a product enhancement idea to add this functionality.
Within that product idea, there are a couple of work-arounds and I used to use one of them that let you do a "same ref" attachment but I can no longer make that work (i'm on Creo 4, M090). Not sure if it's just me or if that work-around has been "corrected" (for lack of a more crude word).
This is a functionality that needs to come soon. While we are waiting, there are a few workarounds:
If you go by option 2, you could sync your layer with a simp rep by creating a simp rep driven by a rule to exclude everything on the layer you created. Unfortunately, as far as I know, you cannot create a rule in a layer to include everything excluded in a simp rep (which is weird, because when you create a rule-driven simp rep you can create a rule based on what is excluded in another simp rep).
The enhancement request has been around since 2013 and it was a problem long before that.
Waiting is probably not an option.
For me, layers are not an option since my primary usage of Simplified reps is for "Large assembly management" and layers only affect visibility but the models are all still loaded in to memory.
Using simplified reps for "product variations" is not how it was intended to be used and may be why PTC has never implemented a fix.
Yes, we are also working with large assemblies so using layers will be an issue. so what are the way around as of now? it looks like edit attachment with same REF is one of the option, is there any other work around.
My number 4 in the list above is a workaround some people use. Not sure if it's too much of a hassle for you. Let me know if you want it explained in more detail.
Can you explain that bit more. since assembly we are working is very large. so i may not able to open up each part and add parameter. But please detail it and i can look in to it. Thanks for the help.
EDIT: I first mistyped the report parameter as "&asm.mbr.POS". It should be "&asm.mbr.cparam.POS".
Sorry about the delay. Been out traveling. Here's what you need to do:
Thanks for your reply. in my case the list of components are massive. the same component may be used in many other projects. since components are more it is difficult to add parameter for each.
I always use option 3: Component Display.
It is so easy to do it because you can select dozens or a hundred parts at one time and hide them at one shot.
this may help you
Consider that for this kind of business need, the suggestion from @JS_9824412 is the one we propose as well, as documented in article 31065 (confirming as a current limitation that usage of a single unique repeat region cannot be the starting point of BOM balloon values being produced and mantianed in different views for multiple simplified representations in assembly drawings)
In other words, create BOM Balloons for all components (starting from Master Rep), and then use Search Tool for a quick and easy access to Blank Components in Views.
Just trying to help a bit further here. Not an ideal approach, I agree, but I do not see any better way to do this, due to the current limitation officially documented in above article.
There was a mention in this idea that propagating combined states to the drawing might help alleviate this problem. If so, could the idea be boosted since it clearly has multiple applications?