I have a model of an enclosure and a door on sheet 1. The BOM
for this model is also located on sheet 1. On sheet 2, I have a
more detailed view of the door only. I want the balloons on sheet 2
to reference the same item numbers that are referenced on sheet 1.
How can I accomplish this?
How can I accomplish this?
I have the assembly linked to the BOM. I have also sorted the BOM to keep the "Description" field in alphabetical order.
All is well on sheet 1.
Sheet 2 is another story. When I "Auto Balloon" the door assembly on sheet 2 (a sub-assembly of the main assembly on sheet 1), the balloons do not match what is on the BOM on sheet 1.
This is such basic functionality. I cannot believe that I don't have the option to link the entire drawing (every sheet) back to one common BOM. Or can I?
Yes, I do have a seperate assembly file on sheet 2. But, it is the same (sub)assembly used in the main assembly file.
Untill then if you select the bom to follow the assembaly order you should be able to get the boms on sheet 1 & 2 to match as long as you do not try to change the order of items in the bom.
The only purpose of an item number is to be a quick reference locator, between a line in the BOM and the drawing views, for parts which are shown on the sheet. No more, no less. They are not intended to cross reference parts between sheets; that's what part numbers are for.
When shown on its own sheet, a sub-assy is a distinct entity from the upper level assy it is used in, and should be treated as such.
However, if you really need/want to do this, you can insert the upper/top level assy into the drawing sheet, and then hide all but the needed parts. The BOM will then have to be massaged to also show only the needed parts.
Edit::: A config could also be created at the upper level which hides the uneeded parts.
There is a need to do this kind of thing in certian instances. When you work for a company that does a lot of custom job shop work most of the parts you use will not have a part number. Especialy when working with steel cut for weldment applications. You wouldn't want to give each peice of steel its own part number. You may give the assembly its own part number but not each part.
I agree in fact I do not subscribe to the Item # in the BOM. I seen where a part was added to an assy. and moved around in the order and all of a sudden det 14 is now det 27. It much nicer to add a Custom prop and give it a # then make that the Balloon and BOM #.
I agree with you on the purpose of the Balloons. They're a reference between the BOM and the part or sub assembly.
However the user should not have to jump thru that many hoops when working in a multi sheet drawing of a large assembly.
When ballooning a detail of the assembly or sub assembly on subsequent sheets I want to be able to specify which BOM to reference.
I generally only have one BOM and it's usually on sheet 1 with the top level assembly views as it's reference.
This may be coming because this option was alluded to in the survey that Sal Lama posted recently.
Regards,
If there is a need for a sub-assy to be detailed separately, why are the parts being 'Item Numbered' at the upper level? The sub-assy is all that need be itemised at the upper level, and the BOM item line should point to the sheet the sub-assy is being detailed on.
What you have described is what I have resorted to doing.
What I'm trying to do is have only 1 BOM ( with indented sub assembly's ) on sheet 1
Regards,
EDIT: I think that many BOMs use to much real estate.
I guess I should explain more on what I runn into here and If you have a better way to do this let me know. We build a lot of custom catwalks and platforms at my company. We will get an order to build a catwalk or platform that will have about 20 to 30 different cut steel p[eices in it. We use the first page to show the assembaled assembly with a bom and ballon details for all of the parts. The next page is where we detail all of the parts. I ussualy insert a view of the assembly of to the side and insert a bom. Next I ballon all of the parts on the assembaly view on the side and place a note under each part and link it to the ballon on the assembly so the right part number will show up. The problem I have is that if I or anyone eles changes the order of the parts in the BOM on the first page the second page will not match. I know 2009 will have BOMs in the assembaly and that will fix this problem but for now I have to be carful and constantly double check to see if the bom's match.
Kelvin and All,
I'm going to jump in here and say that I have to agree with most of what Kelvin is saying. I know there are certain circumstances where something out of the ordinary is required or seems to be required but these should be the exception, not the rule.
Under this particular topic, some of the things being requested are "wants" versus "requirements" and I'm afraid I'm seeing this more and more. This to me is not a good sign.
Now before anyone gets all defensive, I'm not picking on this particular topic, there are many/plenty of others that fit the bill.
Many of the things that people are asking for do not meet ANSI, ISO, DIN or any other standard. Because of this, how can SolidWorks decide on what to provide (functionality) and how to provide for it (capability).
Many of the things that people are asking for are easy to do in a 2D world where nothing is associative and you basically document anything you can think of using any method you can dream of; However, when you are talking about 3D where models drive data on drawings and the data is bi-directionally associative and paramatric, then the issues are much harder to solve.
Dear SolidWorks,
Please focus on providing the functionality & capability that meet/follow existing standards & specifications such as; ANSI/ASME, ISO, DIN, JIS, etc.
That's all I want!!!
Thank you and Merry Christmas
OK, I agree with what you have put forth. It seems logical. However do you know of any requirement in the standards you list that would frown on a single indented BOM on a multiple sheet drawing?
I ask you because you seem to be most articulate in this area.
EDIT: Here is one after thought. I wonder how much effort is being put into upgrading the standards to comply with the expanded capabilities we now have with this evolving software?
To me it's the old law verses spirit thing.
Regards,
I have always used the BOM-per-sheet method so that any single sheet can be issued and will have all pertinent information on it. If all the information is on the first sheet only and it is not available (for whatever reason) the rest of the sheets become just pretty pictures.
Neither regular BOMs or Weldment Cutlists have a way to keep the bom the same on both pages. I guess I will have to wait til 2009
If you created a different configuration for just the door, then you can link the view of that configuration back to the BOM on sheet one by right-clicking the view and going to 'properties' and then selecting the BOM in the 'keep linked to BOM' pulldown menu.
The the behavior here depends on you have you have part configuration grouping set up.
Now, if you have created a different assembly for the door and have inserted that on sheet 2, there's not much you can do to keep the bubbles in synch with the BOM table. you can insert this assembly into your parent assembly and change to BOM to show an indented parts list but that takes some setting up.
As somebody who does multi-sheet drawings (because we only have 11x17 printers), I'll argue that balloon numbers are significant beyond just a quick reference, particularly if your drawings and MRP system have to agree.
John