Deleting a BOM Item

On revised drawings, I typically see the item removed or changed and then the removed or changed item area now blank or changed is bubbled to indicate a change.

Remember to make a notation in the title block area such as "Revision 1" when you make changes.

A separate narrative in the form of an addenda is usually issued with the revised drawing to call out the changes.

As each change (revision) is made after the issuance of a previous drawing, update the revision number.

In this case, item numbers 9 and 10 should remain (with text or symbol removed) to further indicate the deletion.

I've seen BOMs marked to indicate certain parts are used (for example) in an assembly for revisions 'B Through H Only'. --Rather than deleting the item entirely; sometimes an 'oops' happens and the decision is reversed and the item is then later used again on revisions 'M And Higher'.

Assuming we are talking about a parametric model ...

Doorman comes closest. If model content is generating the schedule content, and the parts are deleted from the model, their listings in the schedule will simply disappear. What will happen to the numbering of the remaining lines in the schedule depends on whether the schedule generates its own line numbers or draws its line items from parameters in the modeled parts and orders its listing by those numbers. A kludge (unpleasant side effects likely) would be required to add dummy lines where the deleted parts were, or explain the missing numbers, or use the "strikeout" technique.

If the schedule is displays other characteristics of the parts, Doorman's suggestion should be augmented to include altering parameters of the deleted objects to reflect their "not used" status in the schedule. An alternative I like would be to edit the deleted parts to render them invisible and disconnected from the rest of the assembly but to leave them essentially where they are, and then edit one prominent scheduled parameter to have a value of "NOT USED", and the other scheduled parameters to have values of "-".

As already suggested, changes at the schedule and any drawings which showed the deleted parts should bear a numbered revision tag and the title block on sheets where those drawings appear should indicate the date of the revision number with other info per office conventions (ie: Date, Description).

Hi Rotag, as far as I'm concerned, we are using at the plant I work for, SolidWorks.

When you make an assembly, you put together several parts, and each part has its own name/description. That name/description will appear "automatically" in the B.O.M. So, you'l have to delete that specific part from your assembly and the B.O.M. won't show it, it will show a blank row, or if it last or first in the list the numbers will update automatically.

This is the case with SolidWorks, it may be the same case with Autodesk's Inventor, but I'm not using that sw.

We use Catia v5 here.

When a BoM is updated, and deleted items are removed from the 2D "paper" drawing - it's actually a pdf file that the rest of the company can read. Only the Design Office has access to the Catia models.

The change is detailed in the revision block on the drawing.

I have regularly seen notes sayng "Item 4 was QM1845 now QM 2274)" or "Item 4 REC123 deleted, Items renumbered". I don't fly Catia, but have spoken to one who does....

The parts list that appears on the drawing is generated from the model when the designer requests (kind of a manually triggered automatic function) and the numbering is based on the order of parts in the model tree. The designer (and checker) then have to ensure that the bubbles on the 2D drawing match the parts list numbering.

We don't stored previous issue level models, but do keep previous issue level pdfs, so the changes can be traced back.

There should be a Design Request Form which records more detail about the change and its reasons. A note is added to the Business System part record that usually has the DCR number and the responsible party's name listed!

Hope that makes sense...

We use Autodesk Inventor & our process is much as English Rose describes. When parts are deleted from the assembly model they disappear from the drawing BoM. You could make the parts invisible in the model so that they still show in the BoM but if the decision is to remove the parts why would you leave them there? In Inventor the drawing item balloons will automatically renumber when the BoM is refreshed.

We note the Drawing Change number & brief details in the drawing issue area & archive a PDF copy of the old drawing for traceability. This method satisfies the requirements of ISO9001.

And TS16949

By "drawing BOM" do you mean bill which is written on the actual drawing itself, or a bill which may exist as a seperate document? Where I work, we do not put bills on the actual drawings typically - we generate a seperate document. If we have an engineering change order for an assembly, we also generate a document change order and simply delete items from the BOM - the change order contains the pertinent information as to what was removed and the rev number (or letter) will be identical to whatever the new drawing rev is. ECO's, DCO's, etc are all linked to the drawing files through a central database. Depending on what industry you are in, and what country, you may have certain regulatory requirements and standards regarding this issue.

The OP specified that this is the drawing BoM & relates to a 3D CAD system.

What Nigh said...

And our drawing BoM is a reference for human operators. The CAD system is linked to the Business System. When the products are exported from CAD to BS, the BoM is created in the BS and this is what is used to order from suppliers and created shop orders (work instructions).

Any drawing update necessitates an re-export tot he BS to upissue the BoM. Issue levels are also associated with this BoM and tie in with the drawing issue levels.

One typical method is to include a revision level in the CAD model file name, assuming the model name contains the part number. This revision level links back to the documentation requesting/authorizing the change. Assuming the BOM is tied to the CAD model, this version of the BOM is also saved with the same revision level. This method allows for a tracked implementation date of change (tracking the revision level), as well as maintaining the history of the model with the previous revision level. The revision level is typically an appendix to the part numbers and assembly numbers. By preserving the history in seperate CAD models, the evolution of the parts and assemblies can be recalled at any time.

If the BOM is not directly linked to the CAD model, then the file name for the BOM should also contain the same part number and revision level as the CAD model.

This also has the additional benefit of having records of planned implementation dates, should it become necessary to review the history of evolution.

Simply put, all documentation relating to a change should all carry a thread connecting them together. Usually this would be the request/authorization document number, which itself would record the parts and models affected and their revisoin levels. This is a gross over simplification of PLM (Product Lifecycle Management), but gives you an idea of what is typical.

I too thought Bill of Materials.

In my company (and Nigh's by the sound of it), the B0M is enumerated on the technical drawing, so all information is available on one (haha) sheet. As I explained in my last post, the BoM also exists as an entity in our Business System...

Every company has it own drafting pratices, but most revise drawings like the U.S. military. You make whatever changes are needed without highlighting or otherwise indicating what was revised. Briefly describe the changes in a revision block, usually located in the upper right corner of sheet 1. The whole set of changes is called revision "A". If you revise the drawing again some time later, that is revision "B", and so on. Any bill of material (i.e. parts list) is normally considered part of the drawing, even if it is actually a separate document. Because electronic drawings cost almost nothing to store, the modern pratice is to keep a copy of each revision on file in pdf format. If the changes are extensive you may also want the keep a copy of the model, but some CADD software makes that difficult.

Industry standard in the Architectural and Civil Engineering world (as I know it) is to draw a "Cloud" around the revision(s) coupled with a corresponding "Triangle" with the appropriate Revision Number inside of it (next to and outside of the cloud line)....the Revision is always described in the Revisions block which resides inside or close to the drawing sheet Title Block. Usually each revision is dated, initialed by the engineer making the revision, and countersigned (initialed) by the supervising engineer, usually a PE (if any).....that way all changes are delineated from cradle to grave throughout the project, and who was responsible for each. It's a checks and balances approach to engineering QA/QC, as well as a way to prevent unwarranted "Errors & Omissions" which could lead to potential litigation if there are problems later on, such as failures etc etc etc.

Thank you to all for your comments and references.

Yes, BOM is Bill Of Material (parts list) of the items (parts) that are included in the assembly shown on the drawing.

My industry is Tunnel boring / Mining. We use Solid Edge here and the CAD files are managed with Teamcenter (PLM). Our drawing changes and notifications are created with an Excel form they have created, a PDF is created of this Excel form and distributed to managers associated with the particular machine. We list changes that were done for the revision and make separate notes to the purchasing and production control department for each drawing change as to what changes were made and any special action that those departments may need to do. On the drawing itself, the revision block lists changes that were done on the revision and we place small triangles with the revision number inside next to the area where the change took place as well as next to the BOM if applicable. With the PLM Teamcenter, there is a PDF created with each drawing at that revision level and preserved as well as the drawing. The models are there however I believe one can not open past revisions and see the geometry unchanged.

Our current system does not drive the "Business System" yet, but I hope this starts to happen with the new upgrades the IT team is working on. What a concept! There is still too much manual and redundant data entry throughout the current processes in place here to put a part or assembly into the Business System and purchasing ordering parts and assemblies. In the future (HOPE), the product (parts and assemblies) would feed the Business System and they can create a push-pull environment. (HOPE, as it is possible with the applications we have)

So, back to the issue of deleting a part from a 3D assembly model and updating the drawing revision and BOM. I have been at this drafting career for a while, starting out with the good old drafting board, T-Square, pencil and ink pen. Took a change for a while but been back for quite a long while now. Back in the good ole days, I can see where one would want to draw a line through an item on a BOM while making a revision and carefully removing lines that showed to part on the drawing. This was more practical in most cases than re-drawing the whole thing over again and making notations in a revision block. The purchasing and production control functions was on ledger paper and very long lists. It was lined-out on their documents as well. That is all perfectly understandable back in the days of paper and ink.

As others have mentioned, when a part is removed (deleted) from a 3D CAD model it is gone, there is no more data carried within the 3D model files and the drawing is updated and this part is gone from view and disappears from the BOM which is "automated". The BOM is generated automatically from the CAD model. So when I removed items 9 & 10 they would disappear from the drawing views as well as the BOM. The item numbers would update and fall in a sequential order. But the CAD manager and current company procedures is to have the BOM list item 9 & 10 as DELETED ITEM. They created some 300+ 3D "parts" with no mass or material with item ID and names of DELETE-1, DELETED-2..DELETED -9, DELETED-10....DELETED-300. We are supposed to replace the 3D parts in the assemblies where we are deleting these part with these DELETED-9 and DELETED-10. One has to make sure that they use the same -number as what was used for an item number on the previous BOM for the DELETED-## so the new revised BOM has that DELETED part showing up in the item number that matches. One has to really go out of their way to set up the BOM to stick these deleted-## in the right spot on the item number listing.

Supposedly, this is so the people that manually retype in BOMs into the Business System know that they are to DELETE that particular item from their system for this particular assembly. Remember I said that we do just like everybody else in creating the additional documentations stating what the revision entailed as well as the revision block on the drawing.

Anyway, in addition to the above, when we sell these machines to our customers, we also provide the drawings in a multiple binder manuals as their finished delivered product. There is someone in the company that their job is to constantly update the manual's drawing package while all the revisions are made in the development process so that the manuals are reflecting the latest revisions. They don't include all of the DCRs or revision change notices, which I would not want.

These machine have over 300,000 parts, maybe even over 1,000,000 parts. The CAD files get hugh and it takes a while to open some assemblies. Adding un-necessary part like these DELETED-## part certainly has an impact as well.

I would like to see us simply delete the parts in the assembly during the revision, update the BOM so it does not reflect the deleted parts, no additional item numbers for these deleted parts, and make the notations in the revision block as to what was changed during this particular revision. All of the paper work, change notice documentation that gets distributed with the revision upon release includes the information of what is being changed and any impacts. When the customer reviews the drawings in the manual sees the finished product and has BOMs that list only what is actually on their machine. Listing Item 9, DELETED-9, DELETED ITEM on the BOMs just does not look right. It also gets the customer to wonder and ask "Why don't I get item 9 and 10 on MY machine?!" "What is item 9 & 10 and why can't I get that on MY machine?!"

When you look at your manual for your washing machine for example, do you see (or expect to see) Item 9 and & DELETED, NOT USED in the exploded view and BOM (parts list)?

Thank you for your additional comments and information. Perhaps in the future I will alter my thinking, sway (I have to follow procedures here for now anyway) company policy. I will continue to follow the threads and make additional updates, comments and answer questions. I know this get a little long in the explanations, but I felt it would help give a good picture.

One way (in Inventor anyway, not sure about Solid Edge) to delete the parts but keep the BoM entry would be to create a 'phantom' part in the assembly model. This feature is there to allow you to create parts like oil or thread lock that you can't model but want to appear in the drawing BoM.

I can understand your position a little better now. My previous comment related to my own experiences as an illustrator. Assemblies I was involved with were usually about twenty parts, seldom never more that fifty parts.

I can see the sense in removing items from you BoM and removing the images from the drawing. I would consider this a new drawing, and the sheet should be given a new number (along the line of Windows 98, Second Edition, release 4.10.2222A). I don't think a history of previously released and now obsolete sheets need to be referenced on the drawing; the sheet number itself will tell the tale. Your archive can contain all previous drawings and engineering changes that required the drawing to be reissued. This history does not matter to the end user, he only needs to know what is going on today.

As you say in your explanation, ghost images, delineated part numbers... in your case it makes for too much confusion.

We have 4 different clients, all use Catia V5, and all use different methodology. Some automate the generation of an Excel file which is then manipulated manually. Some do as Nigh suggested an keep the part in the 3D but delete the geometry within the part. This way the BOM will update with numbering order unchanged and a line can be drawn through the deleted items in the BOM. Balloons of deleted parts remain with leaders removed and an "X" is placed on top of balloon. Rev block filled out accordingly.