How to create bom balloons on snap lines ?

[ppandarkar-2]

Hi..

I want to create bom balloons on snap lines, so the BOM balloons should link on snap lines.

I am trying to create it but not getting success. So please can anyone let me know the step by step procedure ?

Regards,

Prashant Pandarkar

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[AmitDeshpande]

Hi Prashant,

You should be able to create the Snap Lines, offset from an object or view, and then drag the balloons to the snap line.

In Creo 2.0, here is what I did:

1. Table > Balloons > Create Snap Line
   • This will bring up the CR SN LINE menu manager
2. Select either Offset View or Offset Object
   • If you select Offset View, select an edge of the view border
   • If you select Offset Object, select an edge, entity, datum, vertex, section or existing snap line
3. Enter the following:
   • Distance of first snap line from the view boundary
   • Number of snap lines to create, if more than 1, then
   • Distance between the snap lines
4. After the snap lines are created, select and drag the BOM balloons to the snap line
5. The BOM balloon will turn purple in color, when it has linked to the snap line

Please give this a try and let me know if you have any further questions on this.

Thanks,

Amit

[TomD.inPDX]

There is a problem with BOM balloons when they are place randomly.

I reported a case a long time ago that I cannot force the balloon back to a snapping grid-point.  If you originally place it on a snapping grid, and always move them with the grid, they will appear to snap to their circle's origin.  In fact, it is simply moving "from-to" between snapping grid points.

If snap lines are working the same as activating snap for the current grid, it may well be that it behaves as I describe above.  Amit's method makes sure you drop the balloon on the snap line during creation.  I am not sure if this will work with existing balloons.

I only recently received a reply to the case.  It seems it was simply lost when an engineer left.  Of course, I got the "works to specification" line so I gave up.  Please let me know if the snap lines ends up working for you.  I like having a clean alignment of exploded assembly views.  And it is really difficult to make sure the "2X" is nicely aligned with the balloon.  In general, "to specifications" is simply a poor implementation.

[TomU]

You're being way too generous with your definition of "to specifications".  I think the reality is much closer to "any behavior not explicitly described or prohibited (no matter how stupid, illogical, or inconsistent) is automatically to spec" (since by definition it's undefined, and therefore not part of the spec.)

It's way too easy to look at something and say, "who possibly specified this behavior", when the reality is, no one did.  Instead, it's completely undefined and therefore automatically "to spec."!!!

Instead of asking, "is this to spec.", QA needs to be asking, "is this behavior logical, intuitive, natural, expected, and consistent with the rest of the software package?"

[TomD.inPDX]

Nice perspective you got there, Tom.  And I cannot find any reason to doubt your logic.

The real truth here seems to be that no one wants to touch the detailing module.

All efforts with regard to detailing seems to be going toward ASME Y14.41 and equivalent for paperless systems.

You know a big cash cow must be asking for this or it wouldn't be happening.

When I go to my precision machine shops, who are leaders in the industry, basically told me that "no drawings, no parts".

So the Creo 3.0 feeble attempt at warming over the detailing annotation section in my view is a miserable failure.

It doubled my mouse clicks and bugs run rampant.  I cannot and will not use Creo 3.0 for detailing.  It is simply too expensive for my clients.

I should climb back off the soapbox now.

[BobSchwerdlin]

The detailing module has needed much work for a very long time.  The implementation of this module in Creo 3.0 defies any logic.  It's as if QC didn't let any experienced users try it out before giving it the OK to go to production.  I can't begin to tell you how many more mouse clicks it now takes me to work on ANY TYPE of notes or annotations.  It's simply backasswards now.  EVERY user in my office has complained about this since we first saw it.  We are not a large company, but all 27 engineers were in agreement on this one.

Also, did anyone at PTC's QC department try the new print routines for Creo 3.0?  it ZSUCKS period!  The white background and yellow object lines and text make it absolutely impossible to preview before printing.  Not only that, but I am constantly having to set the print scale to, Custom and then choose 94% scale.  Otherwise, the edges of the drawing go off the edges of the paper and not only that, it's not centered correctly on the sheet.  In all my years using Pro/E (since ver. 17 SGI-IRIX) I have NEVER seen the print routine so screwed up as it is today.

[dgschaefer]

Agreed. I'm not sure that PTC could have made it worse by instructing the programmers to make it harder to use.

[TomD.inPDX]

I finally got a chance to try this.  It is actually working but the method is not how one would expect.

The answer is that you cannot snap to the snap line when creating the balloon.

Just place all your balloons and then move them to the snap line.  It is working fine in Creo 2.0 and Creo 3.0.

Being able to offset from objects is also nice.  This lets me do angled snap lines typical of isometric exploded views.