BOM - Top Level List required but 3 layers down the Hierarchy Tree

[JIRVINE]

I have a single IRONCAD file with multiple internal assemblies.

I am trying to avoid saving these assemblies out to external files.

I am trying to use a "Top Level List" BOM style but its 3 levels down in the hierarchy tree.

I don't want the BOM to drill down to the 4th level into the individual elements of each steel weldment.

Is there any way of doing this ?

I the only have I have found is to use a "Intented List" BOM style and manually delete out the lines I don't want.

But when you update the sheet, it updates the table again.

[Mike Hatch]

Not sure if this suits you, but its how we do it.

In the main design.ics file we create a "configuration" for that particular assembly in a scene we want in a drawing, for us its usually a drawing # (create gonfig.jpg below), multiple configurations can be made.

You can then select a particular configuration and suppress the (BOM) bits you don't need in the final drawing, suppressing other bits in other configs (layers if you want to call them) if needed for other drawings.

In the design.icd file, create a "Standard View", selecting the "configuration" required for that drawing from the "Part" section (standard view with associated bom.jpg)

Then add a BOM and again select the relevant configuration (selecting a bom.jpg) with "Use Configuration" in the "Assembly/Part" section, your BOM will display the parts that have NOT been "suppressed" in the .icd file config (layer).

Multiple drawings can be done within an .icd file, each if necessary with an individual BOM from the master scene, you will be warned if you try and reuse a particular BOM.

 

 

[JIRVINE]

Thanks for the reply Mike.

I too usually use the steps you have laid out for lightweight sheetmetal design of conveyors. Its very convenient.

For this particular application i have got, I just want to call up the top assembly weldment for a contractor to reference with an item bubble.

And i don't want to show up every piece of flat bar or Angle Iron or PFC on this particular BOM.

But I don't want to save out all the individual assemblies just to get this one drawing for the fabrication contractor.

 

 

[Malcolm Crowe]

This new post (within "Tips and Tricks") regarding combining Assembly and Part levels within BOMs might help you achieve what you're after.

Malcolm

[Guest Bjorn]

On 1/11/2021 at 7:04 AM, JIRVINE said:

I have a single IRONCAD file with multiple internal assemblies.

I am trying to avoid saving these assemblies out to external files.

I am trying to use a "Top Level List" BOM style but its 3 levels down in the hierarchy tree.

I don't want the BOM to drill down to the 4th level into the individual elements of each steel weldment.

Is there any way of doing this ?

I the only have I have found is to use a "Intented List" BOM style and manually delete out the lines I don't want.

But when you update the sheet, it updates the table again.

Did We find a easy way to  solve this problem??

 

[SSIMMONS]

I am most likely oversimplifying what you are asking, but can you just use "expand" and "Treat as part" to get the desired BOM to generate. It is in the part properties under the general tab.

 

-Spencer

[JIRVINE]

3 hours ago, Guest Bjorn said:

Did We find a easy way to  solve this problem??

 

Hello Bjorn,

In IC2022, it has a structured BOM Option fixes the problem by being able to turn off lower layers for the General Assembly but leaving the lower items as parts for the individual drawings.

You can't sort the BOM afterwards so make sure its in the correct order before creating the BOM.

Here is my original issue with the new structured BOM in IC2022.