CREO Drawing Balloons with Different REP

[gkarthikyn]

Hai, 

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.

[StephenW]

Unfortunately it is not currently possible. There is a product enhancement idea to add this functionality.

https://community.ptc.com/t5/Creo-Parametric-Ideas/Allow-BOM-Ballons-from-Master-Rep-Repeat-Region-to-be-displayed/idi-p/466852

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).

[Pettersson]

This is a functionality that needs to come soon. While we are waiting, there are a few workarounds:

1. Create several BOM tables (one for Master Rep and one for each Simp Rep) and sync their item numbers. Then hide all tables except the Master Rep one. Downside: Updates risk introducing non-synced items that the designer doesn't notice.
2. Rather than using Simp Reps, create a layer that contains the items you want to hide and then hide that layer on the drawing view. This is often the easiest solution.
3. Use Component Display in the drawing to hide the components you want to hide. I wouldn't recommend this, as it will be harder for people to find how you hid the components, and it's less reuseable (if you want to repeat it on a second view, for example).
4. Use component parameters to set item numbers for all your components, then use these in your BOM instead of rpt.index. (Remember to also change the contents of the BOM balloons to show this instead of rpt.index.) Then, as in the first solution, create several tables and hide all except the master rep one. This will automatically sync all your tables, but you run the risk of others opening your drawing not knowing how it was made.

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).

[gkarthikyn]

Hai Pettersson, i like the Layer Proposal. we can work out and see how easy it will be for us.

[StephenW]

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.

[gkarthikyn]

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. 

[Pettersson]

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.

[gkarthikyn]

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.

[Pettersson]

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:

1. You add component parameters to your components in the assembly. Call the parameter "FINDNUMBER" or "POS" or something. There are basically two ways of doing this (I use both):
   1. Use the Find tool to search for Components. Select all results, then right-click and go to "Parameters". You should see a Parameters window with all of the components listed. Any parameter you add now is added to them all. You can set the values in this window, too.
   2. You can turn on the display of the parameter in the model tree. Turn on a column of the "Feature parameters" type and enter the parameter name. You can then click on any component to add the parameter and a value.
2. You add the pos. number for each component like this. You need to make sure you don't give different numbers to different instances of the same component, however. So every instance of "M6x35_bolt.prt" will need to have the POS component parameter set to "4", for example.
3. In the drawing, you add your BOM. Instead of setting the index as "&rpt.index", you need to set it to "&asm.mbr.cparam.POS" (or whatever your parameter is called).
4. Then, you need to enter the table properties (select the entire table, right-click and choose Properties" or "Edit Definition") and go to the BOM Balloons" tab. Change the BOM Balloon Parameter to "asm.mbr.POS" (or whatever you chose).
5. Now you can add several such BOM tables, change the rep for each one to the rep of the view you want to put balloons in, and add the balloons. Since all pos numbers are gathered from these component parameters, it's synced between reps.
6. Hide all BOMs except the master rep one that you want to display.

[gkarthikyn]

Hai,

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.  

[JS_9824412]

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.

[rustys]

this may help you

[gkarthikyn]

Video is not helping. Since issue is how to show same Balloon number in different REP. 

[sacquarone]

Hello @gkarthikyn 

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.

Regards,

Serge

[Brndn4]

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?