Raw Material Dimensions to BOM - Automation

[janne_turpeinenKHRUC]

Hi,

What solutions are you using to get raw material dimensions to assembly drawing BOM?

Requirements:

-Drawing BOM needs to update when model is updated

-Needs to be easy to use

I can make a formula that drives an iProperty, which can then be shown in BOM. For example:

For Plate: Dimensions =<Thickness> x <Width> x <Length>

The challenge comes when we look at other raw materials that don't follow the same logic. For example:

For Round Bar: Dimensions =Ø<OD>  x <Length>

For Pipe: Dimensions =Ø<OD> x <Thickness> x <Length>

Writing such equations is not very user friendly, so I assume the solution needed is some sort of macro or add-in that controls how these iProperties are generated.

Please let me know what solutions are available.

[johnsonshiue]

Hi! Before looking to other solutions, have you tried Tools -> App Options -> File -> File Naming Default? There are settings to help set up the default specialized CC part name.

Many thanks!

[janne_turpeinenKHRUC]

Thanks johnsonshiue,

Although I don't see how your answer relates to my question at all, the location you suggested does seem to contain useful settings that might be handy for some situations. Tools -> App Options -> File -> File Naming Default

[dave.cutting]

Hello,

Have you looked at the content centre for things like tubes and bars.

It can be configured to give the part number in the format that you are looking for, although you would need to be running a custom content centre to allow you to make edits.

[janne_turpeinenKHRUC]

I am really confused why the answers are helping me to "set up the default specialized CC part name" or "give the part number in the format that you are looking for". In no point in the original post was part name or part number mentioned.

It is possible that I am not using accurate language to describe the issue as a new user.

[dave.cutting]

I only used the part number as an example.

You can still use the content centre to concatentate all of the fields that you're looking to use (OD x ID x length of the tube) and fire them into a custom iProperty. You could all this custom property Raw Material Size or whatever takes your fancy.

You can then use this custom iProperty in your BOM and assembly drawing.

[A.Acheson]

Hi @janne_turpeinenKHRUC 

Most people use descriptions to hold the description of the material size.Most people take these parts from content center. Are you dealing with something different? Where are your source parts held? Please post an example of how you want to configure the dimensions in the context of the partlist

If your using tube and pipe addin or frame generator or straight from the content center the size dimensions excluding length are generally in the description and length in its own iproperty. If you want all dimensions to be in a description you will need ilogic /vba code or sometimes formulas work as well.  

[johan.degreef]

If you have a tubes or other parts - and the partnumbers are the same, they are stacked up in the BOM. Did you try that? So try to have 3 tubes with different lengths in your assembly and set the partnumber the same if not already. Put the assembly on a drawing and set a partlist.

Better to have tubes from a content center, so that all properties are the same (except length), as you would otherwise have *VARIES* in the BOM.

from minute 15:

https://youtu.be/KSifiDVU7a4

[ampster40]

You are wondering why people are making the suggestions they are when they appear to not be related to what you asked.

In your first message there was no indication you took any time to search on a very common topic and has been asked here countless number of times.

The suggestions you are getting are attempting to steer you towards your end goal.  Work with them, don't question them.

Sorry not much to add here but this is a very common question and has been answered many times before using various methods to get what you are seeking.  Johnson tried to steer you towards something that is already included now.

Good Luck.

[emanuel.c]

Hi @janne_turpeinenKHRUC 

In my opinion you would benefit greatly by using some coding (iLogic) which would greatly improve the speed of your process (defining stock size of components as I understand it) and its accuracy too – you wouldn’t need to enter stock sizes manually and it can be automated.

Setting up the Content Center to suit your needs is useful but relying solely on the CC to generate Stock Sizes is not the best way in my opinion, because:

• sometimes it just fits modeling better to not use CC components, but to draw up a part yourself – think complex sketches, derived or driven components etc.
• using formulas in iProperties requires parameters to be exported, which may or may not be checked for export (requiring extra steps to verify) and which will give you varying styles of formats based on each parts Document Settings -> Units.
• sometimes it is better to modify a component’s size than to begin with a different one. For example I’m using a 2x2x1/4 tube from CC, but needed to modify it later to 3/16 wall. Using size in Part Number or Description is asking for trouble sooner or later, save for the case that it would be linked to actual part parameters.

My solution is a piece of code and an Excel Spreadsheet with some data, which the code bounces off of. The spreadsheet contains for example tables with stock sizes to verify existence of actual stock. You can run the code from a part or from an Assembly level and run through all subcomponents. This is the workflow:

• all parts need a custom iProperty, a Product number: 01 – sheet metal, 02 – pipe or DOM, 03 – angle, 04 – flat bar, 05 – tube etc. This number can be added to each CC part’s family or to the template or later in the BOM. The code creates two more iProperties, “Stock Size” and “Cut Size”
• The code reads the number iProperty and based on its value does a few things:

• For sheet metal, it creates a flat pattern and also writes a parameter “Area” used in the “Cut Size” iProperty.
• For other parts, it requires certain parameters, typically used by Inventor in the CC. For example, for tubes it needs G_W (width), G_H (height), G_T (wall thickness) and FL (final length). For bolts it needs NND, NLG, TPU etc. etc.
• It fills in the "Stock Size" iProperty. For example, if "Product number" is "05" and the necessary parameters were found, "Stock Size" will be: Sq. Tube, 2 x 2 x 1/8. "Cut Size" iProperty will be filled with "FL" parameter.
• All this data is later used in the Parts List in the Drawings.

It works very well for me and I’d be glad to share it, but at the same time I realize it may look daunting or it may be too customized for our workflow and not as usable for yours. I have a feeling that with time everyone sets up their “Inventor workflow” to suit their needs and it looks a bit different for each one.

*** Lastly, a huge caveat! Using iLogic can be incredibly useful. BUT, depending on what you’re doing it may need “attention” here and there. It may throw errors. It may not work flawlessly always. If you’re not prepared to learn the basics then this whole idea here may not be for you…

Here is a snippet of a Part List. Columns "Stock Size" and "Cut Size" is what I was talking about. They are filled in by the code. This is one of the ways it can be 'automated' or at least helped. Thanks!