I have an assembly drawing that requires indented bom, I also need to balloon the parent sub (ITEM 1) but all I can get is the sub-level parts (ITEM 1.1, 1.2, 1.2.1 etc) how can I balloon the Parent?
If you can attach the balloon leader to an item in the subassembly, you'll get what you want. Usually a 2D or 3D sketch entitiy does the trick.
I don't like having to carry such a feature around, but it's been necessary in the past. Helps to give the sketch a special name to help prevent absent-minded deletion.
I use indented Bills of Material to compare the assembly we created to the MRP BOM.
You will notice in the BOM Dialog box under BOM Type, just below the Indented selection, there is a pull-down box. I always choose the "No Numbering" option. This numbers only the top level Subs and Parts. Item 1 will show up as 1 in the balloon.
This is how I need to do the BOM for the USN Shipyard. However, I do need to balloon the Sub assembly as well. The only other work around I for see is a BOM TOP LEVEL only off the sheet and attach balloons to it in the main view sheets, but I then can't use the balloons on subsequent detail sheets of this drawing since it must refer to the large indented bom. Therefore I loose my sub assembly balloon due to defaulting to part level balloon. Did I make any sense at all on this one. Hope I did anyway.
I gave it a try and I can see what happens. I think that the intention is that if you call out all the components of a sub-assembly numbered 1.1, 1.2, 1.3 etc, then they must all belong to sub-assembly #1. A balloon for #1 would be confusing right?
Can the Sub-Assemblies have drawings of their own? Everywhere I have worked puts sub-assemblies on separate drawings. It seems that SoilidWorks is set up to work best like this. Separate page even, each with it's own BOM would work as well.
Well as a matter of fact yes we do.
Here is the way this product works:
We make manufacturing drawings that are shock tested product for use in USN ship applications DDG to be one of these applications.
The drawings for the USN Shipyard must be a COMPLETE drawing. That is an assembly with part s dimensioned and weld symbols attached so that if the event arises in the midst of battle, a machinist on board can sort of reconstruct the product.
Therefore, sub assembly balloons and item balloons must be used. Does this help clear up my snafu? (situation normal all F___d up)
This does seem to be the only work around that I can see. Thanks. I will try this tomorrow at the office.
Another option is to insert a Reference point. I usually select a face in the assembly plus I rename the feature to BOM-00 or DRW-00 or similar. I use a double digit number in case I need more than one. That way the reference point can be identified in the assembly as a auxiliary feature for the drawing. I find this faster than using a sketch. Depends on your preference.
I have been fighting this for some time this afternoon and your post has been a help. For the most part I have been able to get this to work...Kind of. I can place a sketch in an assembly and get it to work. Can I be the first to say it THIS IS MICKEY MOUSE!! Now I come to a challenge that this doesn't work for. Apparently when you use sheetmetal and make it a weldment the indented BOM starts with a sheet of material and the part is a sub-assembly. Then placing the sketch on the part seems to think the sketch is on the sheet and not on the sub-assembly so this trick does not work. I even thought that if I deleted the rows within the BOM the balloons would follow the BOM. It's supposed to right? No such luck Now I am going to have to ponder this some more.
Rant/> 5 years ago I was forced to use Inventor and their BOM was far advanced of the crap we have to work with, It was able to work with this kind of thing. Admittedly this was one of the very few things I found Inventor as good or better than SW on. But since our end product is sending clear concise information to the shop floor or other customers THIS IS A BIG DEAL! </Rant.
Here you will see the BOM before removing any items. The rows in blue have been DELETED, not just hidden. Notice the items with sheet that are sheetmetal.
You would think DELETING something from the BOM would mean that it is not included in determining balloon sequences. I guess not. Now I attempt to place a sketch on a sheetmetal part, I don't have it as a sub-assembly so the only place to put it is in the part, right?
The only two ideas I have are either to dumb text the balloon number in but I don't want to do that since the next person to work on the drawing might not be me and would expect the balloons to change with the BOM like they are supposed to. Of I could chance the parts to not be a weldment which they are only because I keep hoping that someday we will be able to use the cutlist bounding box in the custom properties for the BOM. Huh, just realized, fight one BOM problem caused by another BOM issue. I must be working in Solid-Doesn't_Works.
OK, it's about time to go home so I will just go and hope I can calm down before working on this again tomorrow.
Well, i just deleted the weldment portion of several of my sheetmetal parts and there is no joy in Mudville today. The sheet still shows up in the BOM so my sheetmetal parts are ballooned as 4.1
Come on SW! Get with the program!
Now I just have to wait another 10 months for the Top 10 again.
Yes, I noticed the same thing as Jim. I don't know how most people balloon their sheets, but I thought ballooning subassemblies was normal practice. I don't know how long Solidworks has been around, but this should have been available from the beginning. Only been using Solidworks for a few years, but I don't really have much good to say about it. Very grateful for all the help on this forum though!
... Here is one more workaround that I have used, but it is a pain... add a view on the drawing, RMB, properties, then "link balloon to the BOM on another sheet", then change the scale of this view to 1:20,000 so it is basically not visible. I haven't used this method to connect a leader to the part, but rather used a balloon without a leader and a description using a note to identify the part, but I imagine it could be used in other ways.
I do have same question.
I want to be able to show with balloon parts and assembly inside sun assembly.
Hi William ,
Please find attached it worked for me.
I did think about that, but I needed to be able to control the general area where the balloon attachment is, so the sketch in the assembly sub I am wanting works out quite nice. Takes a bit more planning though, but all in all is both are decent work arounds. Thank you for the good screen shot describing the method. This will help others.
You can overwrite the text in the balloons in the Balloon Settings by selecting "Text" in the Balloon text: pull-down menu. These balloons must be reviewed, however, whenever there is a change to the drawing because they will not automatically change as the BOM changes.
As you suggested we can use text but it is manual, every time we replace a part have to remember update the text.
Try this, I've had some success after reading your posts.
Right click the sub-assembly you wish to balloon in detail and select 'dissolve' & you are done.
You can now balloon both parts and sub-assemblies of the main assembly & parts within the sub-assembly of the main assembly.
Does this dissolve the subassembly in the drawing only, or does it pass that on to the assembly? I can see where this would cause MAJOR problems in the models if someone in the drawing dissolved the subassembly and then used the save all option, but then if they didn't the drawing would be all messed up the next time it was opened.
It's easy. First you need a BOM that shows your assembly or component. Now insert a balloon to any of your components.
Select it and hit CTR-C (makes a copy). Now go to your feature manager and browse to the assembly or component you want to balloon.
Click & select the origin then hit CTR-V and the balloon will show the index of the origin owner. Works for any component. Hide the leader if its in the wrong spot. If you need the leader go into your assembly and add a reference point in the area where you want it to appear in the drawing. Go back to your drawing, again select the reference point in the feature manager and hit CTR-V.
Interesting, I will have to give that a try. I think I would have a hard time remembering if I didn't do several the first time or two.
I see your point but no, it only applies to that specific BOM.
I use it because I have a spare parts BOM for my products, some of the spares reside in sub assemblies so I need to easily balloon them, this is the method I use.
There is a method to do this globally , it can be found in the Configuration Properties as shown below:
This option will show the assembly as 'dissolved' in all BOM's in which it appears.
This is great to know! I have used Promote a couple of times and the ALL is a problem as I usually want the Subassembly to show as a sub.
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