this may sound like a dumb question but it is peaking my interest. when i am ballooning something in an assembly it gives me the option to put the “item number” in the balloon. how does sw assign an item number and what is it? the item number always seems to correspond with the detail number i assign to our components somehow. can anyone give me some insight on this?
Chris Serran 7:40 am on January 14, 2009 Permalink
The Item Number of the balloon corresponds to the BOM item number. The order of it is pulled over from the order of the parts in the ass’y tree.
If an item is tagged as “exclude from BOM” in the properties, SW skips that item in the numbering scheme and goes to the next.
However, you can manually change the order of the BOM in the drawing. Click in the space just before the item number and the BOM will “expand” and show the cell labelling. You can grab the cell number and drag the entire row up or down.
Hope that helps.
sldprt 12:54 pm on January 14, 2009 Permalink
in a BOM, hidden parts are included in the number order, in the order of assembly tree. if the part is suppressed, the BOM will skip these parts without skipping numbers. This is important to know if you have different configurations of an assembly, and want multiple sheets to show same numbering for same part. you need to hide components instead of suppress, in each configuration.
sldprt 11:13 pm on January 15, 2009 Permalink
While I was teaching people SolidWorks for 2 years, They would also say “this may sound like a dumb question but”. I would always first respond there are not dumb questions. Or if after they say I know it’s a dumb question, I would say I have heard worse.
It is peaking my interest. Is how I can show this is far from a dumb question.
“when I am ballooning something in an assembly it gives me the option to put the “item number” in the balloon. how does sw assign an item number and what is it? the item number always seems to correspond with the detail number i assign to our components somehow. can anyone give me some insight on this?”
I will try and answer the question “some how,” by explaining the internal workings of SolidWorks API.
The Top Level Object is SolidWorks. From SoldiWorks object you can retrieve everything down in tree structure.
You can request SolidWorks to give you a ModelDoc2 object from ActiveDoc. Modeldoc2 is a Part, Assembly, or Drawing File reference in memory. It is the Normal state of a file. A part file on its own only has a normal state.
Assembly introduces a word you used, “Components”. I know these as Comonent2. When I first discovered component2 I was excited, but I was tripped up pretty bad at the complexity at first. In order to get a Component2 in memory, you need to ask for the assemblies Component2 through its Configuration.
When you have the assembly Component2 Configuration, each Part, and Assembly are in the state they are in, because the top level Component Configuration holds that information. This includes everything display states.
This is were it gets very weird and complex, I will try to make a simple example. Lets say we put a bunch of assemblies inside one another a whole bunch of times and then put in one part file at the bottom.
Assembly\Assembly\Assembly\Assembly\Assembly\Assembly\Assembly\Assembly\Assembly\Assembly\Assembly\Assembly\Assembly\Assembly\Assembly
\Part
Each level of assembly will show the part in its default open state of its configuration. If we color the part at the top level assembly, it will be stored inside the assemblies display state at the top level, and not the part file. So lets say we open the next level down assembly. It will display the part in the normal state again. You can then hide the part at the 2nd level of assembly, and open the 3rd level down assembly. You will see the part is not hidden anymore. This is because the information is stored different at each level of assembly, and stored in the assembly files display state for its configuration. Might I add we always have at least one configuration, be it even Default. Now if you open the top level assembly, it will not be hidden, even though the 2nd level hides the part.
This is an organised structure, but allows for a complex spider web of views.
Now to answer how this relates to ballooning parts. A balloon will only attach to a part if its is shown, unless you cheat by selecting its origin inside the feature manager tree, and selecting origin is the only way to select an assembly. The component2 in the drawing view will balloon in the order that it is in the tree, and ignore only suppressed parts, and exclude from BOM checkbox. Hidden files are included in the numbering and order of numbering, even though they are hidden, and the BOM will not show as a line number, and will skip over them in order.
It’s the configuration of versions, and combination of display states for each configuration, at each level of Assemblies, that makes the web of confusion. The best way to make sense of it is to think of the lowest level part, and work backwards. This means opening the part, then open the assembly the part is in, then subassembly it is in, and so on.
Everything I have said he is what a component is, visual states, Hide, show, suppress, nothing more. All stored in each configuration at each level off assembly, cascading down.
Modeling, custom properties, sketches, features… these are all derived from Modeldoc2 just like Component2 is derived from Modeldoc2. Component2 exists to facilitate assembly file storage of Model States.
For ballooning this makes a lot of sense. When you balloon something, the Component state for the configuration of its drawing view is shown, and a BOM would display the configurations hide show state for the top level assembly of the drawing view. If you add the option to show custom property with the balloon item at the same time. In order for SolidWorks to retrieve this value from the Component2, it must ask the Component2 for its Modeldoc2, then ask the ModelDoc2 for the Custom Property Manager.
For people that have grown with SolidWorks over the years, it now makes sense why custom properties was an enhancement that came over more recent years, when including them with balloons.
At any note, even if you are not a programmer. Reading the SolidWorks API help file will clear up how things are related in the interface. Pretty much everything you see and use in SolidWorks is available inside the API.