B.O.M. balloons showing "ref"

[SYNDAKIT]

Is there any possible way, or work-around, that would allow me to place more than 1 bom balloon without it showing up as a "REF"?

Suppose I have created piece 'f' balloon, now when I go to do that piece again in a detail, it shows up as "REF"?

I would like to be able to call out the piece in as many views as I would like without the balloon becoming a ref. Is this possible?

The goal here is to have both pieces look like "r" not the one with the circle and line below it.

This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

[neomechanikos · Accepted solution]

If you have more than one of the same component in an assembly drawing then you can redistribute the balloon quantity and add balloons for more instances of that part.

If you are calling out the same component more times than the quantity in your BOM, then you'll have to add a custom balloon symbol that matches your balloon scheme. It's usually frowned on to do this as the number of balloons is usually an indicator of quantity...hence the reference balloon. Furthermore, if the number changes in the BOM structure your symbol won't update.

[SYNDAKIT]

thank you very much. I had a feeling that's why it wouldn't let me do more than the quantity. also the context is large weldment drawings. do those rules of quantity and actual number of piece marks hold true in the weldments?

[neomechanikos]

As far as the software is concerned, a strict relationship of part to balloon always holds true that I'm aware of. But what you consider as identical parts may differ from what the software considers is identical. For instance, if you have assembly cuts it may consider the part unique compared to it's identical "part" because it has been altered at the assembly level.

This has been a headache in the past on large weldments I've worked on. Consquently a two-tier approach to large weldments was developed to keep machining operations in a separate model from the weldment assembly. So, an assembly of large parts and weld features was merged into a single part file upon which machining operations were modeled in. It's both representative of the real world part and keeps the welding drawings separate from the post weld machining drawings, as it should be. Finally, BOM issues and assembly cut problems went away.

What do you hope to accomplish by having duplicate balloons?

[SYNDAKIT]

I would like to display the piece marks in many views and across many sheets of the drawing.

[neomechanikos]

Here are five ways to do it that I can think of, they aren't elegant solutions and they are all manually adjusted except #4 and #5:

1. Create a balloon note(Creo 2.0). May have to add a space before and after the number to get a matching balloon size.
2. Create a custom balloon symbol.
3. Create simplified rep copies of the master assembly and a BOM table for each copy, match the BOMs, move the BOMs off the printable margins of the drawing. Highly inadvisable.
4. I haven't tried this method...use the reference balloons but place an offset filled square over the "REF" and change the line style to a color that doesn't print...use a pen that doesn't print. I don't know if this would work or not. At least the number would always update correctly and automatically.
5. Just get everyone accustomed to seeing a reference balloon.

I recommend #5.

Edited: fixed a few typos and errors.

[SYNDAKIT]

ha ha thanks.

very creative!

#5 for sure

[ptc-5232095]

Great scoot arounds - I'm constantly hounded by questions "why is this like this when {enter any CAD system} can do it?" - I can't answer after 14 years of using the software - this is still an issue.

Creo3 may change all this?!! (don't reckon so)

I admire your energy to bridge the short falls of the software, where's the backup?!!

Cheers

Nick

[ptc-5232095]

I'm suprised it's this complex.

A quantity balloon shows the quantity number of that component in a balloon, a standard balloon just shows the component. On any other CAD program you can have a standard balloon on a component as many times, anywhere. If using quantity balloons then they will be limited as you are counting them out on your structure. Reference balloons! In my ten years drafting - never heard of them!! Give me a break! Are we inventing drawing here?!!

Creo - needs to keep this in touch to stay ahead - same as the pathetic weld symbolds (unuseable since proe20), rendered section views,printer setup and not being able to take scale text of detail views (to name a few).

Rant over

nick

[ptc-5232095]

I found you can switch it off using the table properties/bom table and taking default ref off.

Hope this helps

Cheers

Nick