Item ballooning non-geometric parts

[rossob]

Is there a way you can add an associative item balloon in a drawing to a non-geomtric part that has been added to an assembly? I have a few items in my assembly, like oil, counterweights, etc that are non-geometric parts, which I still need to item balloon to show where they go.

Ross
NX6.0.1.5 WinXP SP2
TC V10.0.2.4
SolidWorks 2007

 

[jerry1423]

yes ...

Insert > Symbol > ID Symbol > Then pick a screen position for yout arrow (just don't pick a solid edge on the drawing) ...
> If you want an arrowhead you need to click first where your arrowhead is going, then (with you right mouse button still depressed) click where you want the ID symbol to go.
> If you do not want an arrowhead then simply click once at a screen position

You can attach these ID symbols to another drafting enitity by clicking on it with your right mouse button and picking "origin", and make sure "associative" is toggled on - then use the bottom icon, you will need to play with the values to get what you want.

 

[rossob]

Hi Jerry, thanks for the reply. I'm not sure if i explained myself correctly to start with. I am not looking at putting an ID symbol to an existing body in an assembly.

We have certain parts which have nothing inside them (non-geometric parts), added to the assembly model so that they appear in the parts list. The problem is even though they appear in the parts list I cannot seem to add an ID symbol to it, which is associative to the corresponding line on the parts list ie. item 18.

I don't want to just manually edit the text to point to the corresponding line in the parts list, because if components are added/subtracted from the model, the item number may change in the assembly tree, but the number will not change in the ID symbol. Hope this clears it up

Ross
NX6.0.1.5 WinXP SP2
TC V10.0.2.4
SolidWorks 2007

 

[hudson888]

Okay well the attribute that you're looking for is a "CALLOUT" and it is an object attribute of the components added to an assembly. You can start by adding an annotation then opening the full version of the editor and look under the relationships tab. There you will find three icons the middle being for object attributes, you click on it and then select the component from the ANT whereupon you'll be presented with a list of attributes one of which is the callout. Callout is a special attribute for item numbers in a parts list. So once you have done this you'll have a text string that looks a lot like <W!36486@CALLOUT> copy that and paste it into the text feild of an ID balloon and you'll achieve the desired result..

I know it seems a long winded round about way to get the desired result, but the case seems to be that it is so seldom required that the software doesn't make a built in accomodation for it.

Anyone who knows an easier way or can comment on NX-6 improvements would be welcome but this was as of NX-5.0.5.3

Cheers

Hudson

 

[jerry1423]

Oh Ok, I am sorry.

This may not be the way you want to do it but you can create an empty UG part with the attributes of the non-geometric parts added to that file, then import that file into the assembly.

I think there is a better way to do it but I am going to have to look into it a little more.

 

[rossob]

Hi Hudson, thanks for that, that was exactly what I was after, but not quite the result I was after. It does point to the callout inside the part, however, I found that the callout attribute inside the part is a TeamCenter callout, which had a value of 320, but the actual corresponding row in the parts list was #18. Not sure if there is a way to point to that number instead?

Ross
NX6.0.1.5 WinXP SP2
TC V10.0.2.4
SolidWorks 2007

 

[hudson888]

rossod,

I'm not in front of a teamcentre installation at the minute so I can't directly answer for you. It will of course relate to whatever is used in your parts list as an item number so if you have an existing parts list with item numbers then analysing the settings for that column will hopefully reveal the name of the attribute being used. If you can find out the name of the attribute the you should with luck be able to use the annotation relationships dialog as I described above to create the require text string for your ID balloon.

Cheers

Hudson

 

[cowski]

Some of the later replies in this thread thread561-189212 may be of use.

 

[ewh]

We use jerry1423's method, except that we include a point in the file instead of leaving it empty. This gives us an entity to anchor the balloon. We also don't import them, but bring them in as components. The main drawback is having to manually edit the qty.

The Edge... there is no honest way to explain it because the only people who really know where it is are the ones who have gone over. - [small]Hunter S. Thompson[/small]

 

[hudson888]

ewh,

Yes I never mentioned earlier that we often create components for the non geometric parts and add them to the assembly.

In the past we would simply add a point to the assembly drawing, assign it with some attributes and edit the parts list to include it. I suppose that still works but for one reason or the other we haven't employed that strategy in recent times.

Cheers

Hudson