Using boms in drawings the right way?

[Safwah]

Heyas, i have a question regarding boms for 2d drawings. The tutorial/helps files give you an idea on how to use them but dont really go in depth on how the program designers intended the process to be done.

 

Atm i just add boms to a view (normally an isometric or exploded isometric) and then drop in a parts list. I then manually edit most of the parts list fields such as description, details, specification. It seems to work for the most part but i run into several problems esp on larger drawing sets.

 

1. Constantly get the message to update the bom list as structured and part only turns off.

 

2. Removing items from the bom can get problematic for other drawings in the set using the same part. Hidding one item requires to renumber the rest which i find effects the same part in a different drawings number. This is caused when i "save bom overrides" but if i dont save bom overrides i get issue #1

 

And a bunch of other problems like going back to one of the first drawings done in the set only to find the numbers have readjusted themselves but kept the original description etc. Which i then need to the the bom process all over again for that drawing.

 

I know theres something im missing to the process but like i said the tutorials/help files really dont give a step by step process on how they intended boms to be used.

 

If anyone can explain the way its meant to be done or a guide out there somewhere please let me know so i can start doing it correctly.

[shift1313]

which version of Inventor are you using?

 

BOM is not something I have to use or have ever played with so I dont really have an answer for you, but I know things like this can be linked to external spreadsheets. Im not sure if that would work in this case.

 

I do know that if you fill out information under the parts properties these will display when you create a new parts list. Even if you change this data it will update in your parts list of your idw file. If you right click on your parts list in the design tree on the left you can edit parts list or edit parts list style. You can add columns from the column chooser that are automatically linked with the part properties. If this all gets filled out and updated, or say you change a part design and use the Replace Part option in your assembly this should all update without additional work.

 

Can you give an example or what industry you are using this with?

[Safwah]

I work in a mechanical field. Conveyors, factory equipment etc. Using 2008 currently. I tried using the ipart propertiest at one point but didnt like the system of it, but maybe thats the problem, boms are supposed to be used by taking information from the ipart properties. Ive uploaded a pdf as an example of the work with how i use the boms.

GF0914047 Tension System Assembly_0.pdf

[MarkFlayler]

First of all, are you saying that you are overriding the Parts List?

Disclaimer: The Parts List and BOM are not the same. The Parts Lists is actually derived from the BOM.

If you research Bill of Materials instead of Parts List you will probably find better results. Try RMB on the View in the drawing and selecting Bill of Material or using the Bill of Material in the Assembly directly so you don't have to change it again later. This is also a great place to modify all the material properties at once and any changes will propagate back to the part files.

[Safwah]

Maybe an explaination of how i do it will give me detail on my process so here goes.

 

1. In a new drawing with views done i normally balloon the isometric view. So add balloons at this point to all parts in the assembly.

2. Go to annotation panel and select parts list and drop a parts list in the corner.

3. double click on parts list that was just placed and edit a few fields, in my case its "details, description, specification". Other fields such as part number and quantity is automatically filled from the balloons.

4. Done and move onto next drawing in the set and repeat process when nessesary.

 

The main problem i get is when opening up a drawing in the future it will have the message. "The BOM view used in this drawing is missing from the following referenced assemblies. The parts list and balloons based on these assemblies reflect the last known values and will no longer update to changes in referenced files."

This causes a few problems like numbers missing from balloons and in some cases rearranging numbers in the parts list. Eg Item 1 with the decription of "test" becomes item 2 with the description of "test" but the balloon itself is still 1. This requires the whole process to be done again.

 

To get balloon numbers to show again though, i double click the parts list and it will say "a BOM view is disabled in the referenced assemby. This BOM view must be enabled to proceed. Do you wish to enable the BOM view." I say ok then close the parts list and the numbers are back. Although even after saving an reopening the drawing it will do the same thing.

 

This is what leads me to believe im going about the ballooning and parts list the wrong way but everything i have searched for there isnt much info on how to correctly produce 2D work drawings to the level i need.

 

All the help file says is "this is how you place a balloon, this is how you place a parts list, iparts do this. Never does it go into the process of how and why you do it the way the inventor programers intended for it to be done.

[DVDM]

I have set up our system in such a way that the BOM is populated entirely by the iProperties of the parts and assemblies.

I have created two different parts list styles, one for Materials, one for Parts. You can create any type of table you like, containing any number of iProperties you want to display.

This way I can model a plate, assign a material (or material standard), assign model parameters to the ‘description’ field in iProperties (6FL x Width x Length), give it a Title (Cover Plate), give it a part number, and have all of these properties populate my BOM. I can use the plate to detail for manufacturing and have the correct material description, and I can use this plate as part of an assembly and have the correct part number. Any changes I make to the model (overall dimensions for example), will be reflected in my BOM. If I make a change to my part, this change will be pushed through to every single assembly/drawing I have used this part in.

 

Now, say that I need another plate that is exactly the same except that it’s made from aluminium. What you would do in your system, is to simply override the material description and the part number in the BOM itself, because visually there’s no difference. Job done. However, as you’ve noticed there’s no longer a link between the line item and the part/assembly itself.

In the system I use, I would save the plate as a new part file (or create it as a derived part, so it maintains the link to the base component), assign the correct material, change the part number, and create a new assembly (save as) replacing the steel plate with this aluminium plate. Because I have physically separate files, I can give them separate descriptions, and maintain their link in the BOM without overriding any values.

Depending on how many and what kind of variations you need you should consider using iParts, iAssemblies, and Level of Detail representations. Also look into using phantom assemblies, so you can create a sub-assembly (Items 1 and 2 for example), use multiple instances of this subassembly in your main assembly, and have all individual components show up in your bom (instead of instances of just your sub-assembly).

[Safwah]

Ahh interesting response and pretty much how i expected it to be used. One thinig that turned me away from using iparts properties was that i didnt know how to make it so it would know the size (2 FL x 30 x 100 for eg). Its appears you have set it up in a way so that its automatic, which makes it very simple to use.

 

Have you also set up tables to use as the material list instead of using the drop in parts list?

 

So basically everything is controlled with the iparts properties in your examples?

[DVDM]

Ahh interesting response and pretty much how i expected it to be used. One thinig that turned me away from using iparts properties was that i didnt know how to make it so it would know the size (2 FL x 30 x 100 for eg). Its appears you have set it up in a way so that its automatic, which makes it very simple to use.

 

Have you also set up tables to use as the material list instead of using the drop in parts list?

 

So basically everything is controlled with the iparts properties in your examples?

 

First, lets make sure we don't get confused with naming conventions; Every part, assembly or IDW has 'iProperties'. These iProperties contains fields with values that can be set to certain values (using Expressions and parameters), and be read out elsewhere (in a BOM for example).

 

An iPart (and iAssembly) is a component that can have various configurations based on values in an embedded table. You end up with a 'Parent' part/assembly (the iPart or iAssembly), and every different configuration is a 'Child'.

 

In the example of the plate, I could make an iPart by making a table with Length, Width, Thickness, Part Number, and probably Material (haven't tried that yet), and simply entering all the values I would like to have for the different configuration.

 

Unfortunately, these values cannot be assigned to the 'Description' field using an Expression. In order to get the material size in the Description field, you will have to add the Description field to your iPart table, and set the correct value manually as text (so 2 FL x 30 x 100, not = FL x x ).

 

I use the Expressions in the Description field, so all I need is a folder with templates containing my most used profiles. (Flats, Plates, EA's, UA's, pipes, etc). When creating a new part I can start with the appropriate template and have all my parameters mapped and ready to go, all I need to do is change the length of my extrusion anywhere from 1 to 6000mm and that's it. This works much better than turning my profiles into iParts, because you can't make individual edits to them because they're essentially derived solids. iParts work well for library components.

 

Also look at the Content Center as it contains a lot of the fasteners and (AS) Profiles, but again with certain limitations when it comes to mapping parameters to create custom parts, and some work required modifying the existing tables to your liking.

 

Sorry, no screenshots this time for clarification, currently not at work

[Safwah]

And do you think this is the way the inventor programmers intended material list to be done? Or is this a method you have developed yourself?

[DVDM]

While it can be extra work this way, I do think this is the best way to do it for our needs. Make changes at a part/assembly level, let them follow through in the BOM automatically.

 

For you though it may be different, depending on your requirements.

Say you have one assembly with 1000 fasteners, and you have 3 configurations where the only difference is the type of fastener used in that assembly (zinc plated, galvanised, stainless). In this case, it would probably be easier to simply change the spec of the fastener type in the BOM, rather than going through the trouble of creating 3 separate assemblies containing the actual fastener, or using different assembly configurations.