Balloon help 1

[fighterpilot]

Really struggling in UG drafting. Placed parts list and autoballooned the drawing. Now I'd like to;

- Create multiple attachment points for the same balloon in one view
- Create additional same numbered balloons in different views.

I'd like everything to be associative if possible. Can't even find a command to create a dumb balloon.

Searching the UG help for "balloon" brought back very little info.

NX6

Thanks...

--
Fighter Pilot
Manufacturing Engineer

 

[JohnRBaker]

While you may call them 'Balloons' and even some of the Part's List dialogs uses the term 'Balloon', in reality they are officially known as ID Symbols.

Note that there's no practical way to add a second Leader to an existing ID Symbol (AKA 'Balloon') other than placing a second one over the top of the first one.

As for adding additional ID Symbols in another view, just go to...

Insert -> Symbols -> Identification Symbols...

...and using the same Type of Symbol as was generated by the Parts List, create as many additional 'Balloons' as needed making sure that the Leader Line is attached to the desired Components. Once you're finished, select the Parts List note, press MB3, select 'Update Parts List' and all of the manually created 'Balloons' will update so that they have the proper ID callout in them.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[fighterpilot]

John,

There is no ID Symbol under Insert > Symbol.

Also, it seems like it will let me reattach a balloon (ID Symbol) to a component that is not the one called out in the parts list. Is that the case.

--
Fighter Pilot
Manufacturing Engineer

 

[JohnRBaker]

It's 'Identification Symbol', as I indicated in my reply (make sure that you're using a Role with 'Full Menus').

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[fighterpilot]

Ah, there it is. My role didn't have everything activated.

So do I just type in the same number as the balloon I want? If so that's not very parametric is it? Will it update if I add/delete/re-sort the table?

--
Fighter Pilot
Manufacturing Engineer

 

[JohnRBaker]

NO, don't enter any value whatsoever, leave it empty. If the leader line is attached to a component, the proper number/letter will be automatically placed in the empty ID Symbol when you perform the Parts List 'update'.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[ewh]

If not using the associated parts list or "smart" balloons, extra leaders can be added.
As much as I hate it, that is part of the work flow here. "Real" parts lists are hopefully going to be phased in soon.

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[fighterpilot]

Alright, that's more like it. So my last issue is it appears if I reattach a balloon point from one component to another it will allow me to do that. Essentially creating a mis-identification.

--
Fighter Pilot
Manufacturing Engineer

 

[JohnRBaker]

That depends. If you change the component that a Manually created 'Balloon' is attached to and then update the Parts List, it will update to the correct number/letter callout. However, those ID 'Balloons' created automatically by the Parts List function, they will always indicate their original callout even if you were to remove the leader line altogether.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[fighterpilot]

/start vent/
OMG this UG drafting package may be the biggest POS I've ever worked with. Something that should have been out the door weeks ago is still sitting on my screen. My kingdom to get back on Pro/E.
/end vent/

Per John's instructions above I can create the ID Symbol. The issue now is attaching it to the correct component so it will populate the item number. It LOOKS like I'm attaching to the component but I assume not because the balloon is not filling in with the number from the parts list. When I move the view it seems like the note just points into space. What is the trick to selecting 'the component'??



--
Fighter Pilot
Manufacturing Engineer

 

[JohnRBaker]

When you're making the pick for the 'end' of the Leader Line, make sure that in the Que/Status line it indicates that you're actually selecting some aspect of a Component (usually an 'Edge'). Also make sure that 'Selection Scope' in the Selection Bar is set to 'Entire Assembly'.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[fighterpilot]

John,

You must have the patience of a saint to put up with all the questions.

When I activate the command an orange circle appears so I just pick a point in my drawing view and then close. Then I double click the balloon and then pick Select Terminating Object. At this point I put my cursor over an edge of the component. Nothing appears in the que line. If I hold down LMB a circle with a line thru it appears.

BTW, I'm working in a full section view if that matters. I get the same behavior in a complete view too.

--
Fighter Pilot
Manufacturing Engineer

 

[JohnRBaker]

When the 'Identification Symbol' dialog opens note thta the Cue/Status line states "Specify origin or press-drag on an object to create a leader". Now I want you to concentrate on the "...or press-drag on an object to create a leader" portion of the instruction by placing, while the 'Selection Scope' is set to 'Entire Assembly', your cursor over the Components of the Assembly and when you see in the Que/Status line that you've highlighted an 'edge' of the desired Component, 'press and drag' MB1, which will cause the leader line to be dynamically rubberbanded. Once the dynamic rubberbanding is initiated, you can release MB1 until you have the ID 'Balloon' itself located where you would like it to be and then press MB1 again, which will place it. Now you can place other manual ID 'Balloons' until you've got what you want, and then you can select the Parts List note, press MB1 and select 'Update Parts List' and the newly added 'balloons' should all be properly populated with ID callouts.

Give it a shot and let me know how it works for you.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[looslib]

I do disagree that NX's drafting is the worse! I feel that the Wildfire drafting package is much worse. The final presentation of a NX drawing is much clearer than any drawing I have done in Wildfire.
I have been fighting an issue for a couple of days with Widfire where the formats pulled in parameters from the model in WF3 but won't in WF4. No changes to the start parts or the format files.

A lot depends on which system you 'grew-up' on versus transitioned to. I started with UG in 1987 and Pro/E in 2001.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[fighterpilot]

looslib,

I'm sure both have the good/bad points. I'm sure the issues here really revolve around the lack of administration rather than the package itself. We typically do just MBD for the product design but the tooling group uses drawings still.

I knew Pro/E like the back of my hand simply because I wasn an admin as well as a user. I'll figure it out in time. I'm just now getting up to speed on the modeling aspects of UG NX.

JohnRBaker always seems to answer any questions I have. John, tried your suggestion this morning. Works perfectly. Thanks...

--
Fighter Pilot
Manufacturing Engineer

 

[64polara]

Try using Catia V5 for drafting sometime. Now that is a drafting CAD program that will really expand your vocabulary.

Wayne Huseby
Drafting Checker
Goodrich Corp
Jamestown, ND 58401

 

[Toost]

Re @64polara,
Are these new words learnt something a non-native English speaker should try learn or are they all proprietary

 

[loworange88]

Hello everyone, I am currently using NX6 natively, and I use a SEED part that has a few things set up the way I want, it is pretty much my only goto for new part creation either model only, drafting views only, or a single file with both model and drafting in same file. I have always just used the Autoballoon feature, and then added manual ID symbols to areas if needed. I have tried the above method with updating the partslist, and leaving the id symbol blank. Numerous tries and slightly different methods I have been unable to get the symbols to display the callout of the partslist. I have started with a fresh assembly, and even opened an older one, I cannot get UG to place text in an id symbol by updating the partslist.

Step 1: start a drafting application -> drop in base view of model.

Step 2: add id symbols to drawing view(tried many different shapes, circle, triangle, split circle, rounded box). Clicked on an edge of components, dragged empty symbol into drafting space, and dropped. Repeat until desired symbols are shown.

Step 3: Insert->Partslist. Dropped parts list onto drafting space. Right clicked onto partslist....update partslist.

Nothing happens. I have to imagine there is a setting somewhere in the annotation settings that is stopping this.

Autoballoon feature works just fine every time, but it doesnt work as described in the above posts.

Thanks,
Mat

 

[cowski]

Try adding the parts list before you create/add new balloons.

 

[loworange88]

COWSKI, I have tried those 3 steps as mentioned in numerous order, so far i cannot seem to get it to update correctly. I even opened an assembly that we recently obtained from our German facility, and it did the same thing. If I add the ID symbols manually and leave the text empty, they wont update. If I autoballon the same view, I can get them to change upon update when I changed the callout menus from the plist annotation style dialog box.

Mat