Difference between 'Base Quantity' Values

[cadman777]

I have a question for all the veterans on this forum.

It's a question about the different uses for DocumentSettings>BOM>BaseQuantity:

Each

vs.

a Unit

I've always set it to 'Each'.

But now that I'm trying to use iLogic, I want to see if there's any value in changing it on a per part basis to a suitable Unit. For example, sheet stock would be 'ft^2', structural shapes would be 'ft', concrete would be 'yds^3', etc.

Thanx for the advice!

[Gabriel_Watson]

It depends on how your procurement/buyer prefers to group the product you are buying.

If you have long bars that are sold in stock size of 1 meter each, you can buy the raw material and cut to length, or add any material together to make up the components (for components larger than the base quantity).
I think this works well with iParts but again, procurement/buying has to be aware you are sending something that is not the usual item quantity.

[cadman777]

OK, but that doesn't make much sense if you set limits on the lengths of your CC parts, b/c then the CC will control the stock lengths.

I guess I should have asked, "What is the PURPOSE for each of the types of 'quantities'?

I always get them mixed up!

[Gabriel_Watson]

Ah, I see what you mean...
Off the top I can see how, if you model a complex mold, you can add a solid that fills the contents to order enough resin, for example (screencast I like to reference when extracting cavity volumes: https://knowledge.autodesk.com/support/inventor-products/getting-started/caas/screencast/Main/Detail...).

I guess you must be creative in the use of units that are not solid (at least not as bought), and think of other fields of application such as architecture (floors bought by area), where maybe one type of tile is bought in inches Vs. another in cm. Or large-scale, a petroleum reservoir requires anti-souring chemicals to fill X many gallons.

I don't have a perfect answer for this, but just exemplifying how it does make complete sense to me. If you just look at procurement's point of view.

[pcrawley · Accepted solution]

I think the "purpose" is so you can make use of the math functions in the BOM editor for calculating information in a model.

• ITEM QTY counts the number of instances it finds in the assembly.
• UNIT QTY knows how much of the 'thing' exists per instance.
• QTY is ITEM QTY multiplied by UNIT QTY giving a total amount of the 'thing' in the current assembly model.

In the case of Frame Generator, QTY calculates the total cut length of each section-size - for example:

• ITEM QTY = 5 pieces of the same section size
• UNIT QTY = 2' (because the document setting "Base Quantity" = the cut length of the frame member)
• QTY = 10' (calculated from 5 x 2) 

In the case of Frame Generator, the frame members are grouped into the same section size and length (by default anyway) - and therefore "QTY" gives the total length of material required to make all the identical pieces (excluding any cut allowance).

If Frame members had "Base quantity" set to "Each", then QTY would be useless.

Without being able to set the base quantity (or UNIT QTY in the BOM editor), I'm not sure there's another way to calculate values from multiple components in an assembly without resorting to parameters, spreadsheets, or iLogic. 

Having access to a wide range of base unit types is therefore incredibly useful if your BOM (and subsequent Parts List and/or exported BOM) needs to provide anything other than "each" (the number of instances in the assembly) - which is the default.

[cadman777]

Thanx Peter, that's exactly what I wanted to know!

Inventor 'Help' got me part-way there, but your explanation structured the knowledge in a useful manner so I can use the BOM to suit my needs. I want to write iLogic rules that are BOM/PartsList related, so this is what I need to change in my setup. This question is a result of careful planning, so the more I know about the down-stream effects of changing my existing methods, the better.

So have you used 'Each' at any time?
And what value (or detriment) did it bring to your work-flow?

I also want to get Area and Volume into the BaseUNIT.

I haven't been able to figure out how to do it 'out-of-the-box'.

Seems like this stuff was designed solely for FG parts.

Is this even possible?

[pcrawley]

Thanks @cadman777 .  I respect your careful planning because I know that getting it right will quickly pay you back.  

The number of unit types is quite limited in the Base Units settings.  It could do with "Area" as an option.  I usually resort to creating a numeric parameter called G_L and making it equal to the value I want the maths to work on.  That way I can use the same parts lists & BOM reports as I use for Frame Generator.  The only downside is that Base Units needs to reference G_L and therefore the units are whatever the default length units are - not the unit required for "Area".

[cadman777]

Thanx for the update Peter.

So you're telling me that there is no way to use this for anything other than LENGTH units, b/c it was designed for FG.

Why doesn't that surprise me?
So today the Autodesk developers are working on VISUAL upgrades, but totally IGNORING the foundational stuff that we've needed for the past decade+. WTF? Just another 'mile wide and an inch deep' improvement that no substantial segment of users will benefit from. Adding this kind of shyt to the program will just further complicate it so they will be even more resistant to fixing the basic stuff down-stream. Reminds me of government edicts. Like my old man used to say, 'useless as **** on a bull.

[pcrawley]

Well, it's hard for me to be too negatively critical because the functions which are available do exactly what I need them to do.  Would I like to see the functionality extended?  Of course, but there's another forum for that sort of feedback.  I think the danger (as with many things with CAD in general) is trying to do too much in one application.  As you said in your OP, there's nothing "out of the box" to do what you are asking for, so customisation is a logical approach to get the outcome you need.

I would be very interested to know how you get on with your iLogic idea - the more I think about it, the more useful I think it would be.  I might even have a go myself...

[cadman777]

It all comes down to the principle of it. Anyway...

Today I ran into a problem when creating a ContentCenter part. After having copied an existing Family to my Read/Write Library, I had to change the sketch to accommodate what I wanted to do. Unfortunately I broke the sketch and had to delete one of the dimensions that was part of the original authored part. So in order to fix it without having to re-author the whole part (b/c it disconnects the Family from legacy project data), I made a tiny iLogic rule to do the job for me. It calculates the inside radius subtracting the wall thickness from the outside radius, and then determines which number to put into the inside radius dimension using logic to make a choice if it's greater than 0 or 0/negative. Worked like a charm, even though the experts in this forum say it's not good to put iLogic rules inside CC parts. I have other tiny rules in some of the CC parts too that fix shortcomings in the program that I got from some guys in the Customization forum.

I'm sure Autodesk does what they do b/c they can count on us doing what we gotta do to get the job done.