Parts List with multiple parts

[ddeck]

I have the formating for my parts list down, but ran into a problem today.

I have 2 parts (LH, RH and are seperate *.par files) dimensioned on the same page. So the first step of the Parts list command asks you to select a View. I can only select 1 view!

Anybody know how I can get the parts list for multiple items in one (and not break the link so it keeps updating when needed)??

Thanks

 

[fredericmenage]

Hi,

you could create an asm file with this two parts in it. Tehn create a view of that asm in your draft (could be outside the sheet if you don't want to print it). Finally, create your parts list using the assembly view.

HTH

Fred

 

[ddeck]

Thought of that, ont thing I don't like about it is that there is 1 more file to keep track of.

Haven't tried it yet, but couldn't you just turn the LH part on and the RH part off in 1 view and then vice versa in the other?
If the part is turned off will it be generated in the parts list?

 

[fredericmenage]

Hi,

yes, it will work. you can create 2 views of the asm but show only one of the 2 parts in each. In your parts list based on 1 of the 2 views, you can get both parts even if one is hidden (just check the options in 'list control')

Fred

 

[ddeck]

Thanks Fred

 

[ddeck]

I run into another problem.

Say I have an assembly of 4 parts. When I create the parts list for the assembly the four items appear all ok. However the system we have in place calls for me to have the first item being the assembly (which has a part#).

So a 4 part assembly requiers 5 lines in the parts lists.

Is there anyway to edit this table (the parts lists) without breaking the link? I wouln't mind opening it and adding the first item and then have the rest of the table be linked to the assembly.

 

[swertel]

You need to create a non-graphic part with the assembly information.

Once you place that in your assembly, it will show up as line item 5 in your current P/L. To get it to number 1, edit the properties of your parts list and go to the list control tab. Turn off all parts except the non-graphic assembly part and hit ok. Update the P/L. Go back to the list control tab and turn on the other parts. Update the P/L again.

--Scott

--Scott

For some pleasure reading, try FAQ731-376

 

[ddeck]

For creating a non-graphic part do i just save a part file with no features?

I guess this would work, but its one more file to keep track of. Anybody else know any other ways? Is there a way to create a Part that is saved within the Assembly file (not a seperate file)?

How do people out there handle parts lists? Seperate documents; automated Visual Basic or C++ add-ins; using parts list command?

Does anybody else every put the assembly in the parts list?

The way we work are numbering is that the part number is followed by a dash number. Parts only ever see -1 or -2, but mostly -1 (-2 is for a Right Hand part).
Assembly start at -1 and go up odd numbers (-3, -5, -7) where even are resevered for left/right hand configuration. Each dash symbolizes a different configuration. -1 configuration might use a certain type of connector/paint/fastner then -3 or -5 but the form, fit, function is not affected.

Its not easy to get your head around and makes for using the Parts list command pretty much impossible.

 

[fredericmenage]

Hi,

I don't think there is any other way than the empty part if you want to list the asm and its components in the parts list...

However, you should try the Reports command (RMB on the asm from the explorer for example) with the option Bill of Material because it lists the asm and the components.

NB: You could then use the 'copy' button, paste it in Excel and insert it in your draft if necessary (no link though...).

HTH,

Fred

 

[swertel]

ddeck,

We use the same P/L philosphy as you. You must be a defense contractor - or doing tool design.

We've put in enhancement requests numerous times to improve the P/L command to allow for matrix type BOMs. Still nothing. We also put some requests in to control the BOM at the draft level instead of just the model level -- add extra columns, for example, that are specific to the draft file the part is used in, not to the part itself.

We've pretty much given up on using the automatic quantity field and just add text boxes in the draft for quantities. We still use non-graphic parts, though, to generate the BOM and fill in all the parts, titles, materials, etc.

--Scott

For some pleasure reading, try FAQ731-376

 

[ddeck]

swertel,

All the managers (and everyone except 2 people) of our small company came from a defense/space company. We're not in that industry today but we are using the same numbering style since most people here are familiar with it.

Could you elaborate on how to do the non-graphic parts? Just an empty part file with the file properties filled out to match the assembly file? Any way to save the part file within the assembly file?

Thanks for the help

 

[swertel]

Yes, the non-graphic part is a .par or .psm file with no geometry created in it. Only the file properties have been filled out and the title, document number, and custom properties are filled out to be the same as the assembly.

Then, in the assembly (.asm) file, we insert the non-graphic part as the first component. We then start "assembling" all the other component parts. We have a non-graphic part for every assembly file just so the assembly shows up in the atomic parts list of a drawing.

--Scott

For some pleasure reading, try FAQ731-376

 

[beachcomber]

You can start item numbers on the parts list/ballooning at any number you like - right click the list then
Properties > Sorting > Start with item number
You could set this to 2 and add the assembly balloon manually as item 1, listing any properties next to the balloon.
I know this will not put the assembly in the parts list but at least you don't have 'dummy' parts in your assembly.

In my experience you don't make the assembly item 1, and I can't really see why it should be, although I'm sure people will have good reasons why it is.
Some places don't put parts lists on drawings - its part of the pdm system.

I do agree with everyone though that there should be some flexibility in the parts list command for adding
user-defined part and assembly information in the draft file.

beachcomber

 

[ddeck]

thanks guys for the help!!

swertel,
since you seem to be using the same Part number philosophy as we are here, where can I find documentation on how its supposed to be implemented? What standard is it?

Also, I've been reading the CM threads and people seem to use the dash number for when form, fit and function (FFF) changes. ie part 12345-1 is where it starts (drawn on drawing 12345) and if its change is only a rev, it goes to 12345-1 B. But it FFF changes then you go to part 12345-3?

Is that correct for the philosophy we are using?
Are -even numbers are saved for right hand left hand parts?
Would you ever go to -11 (ie using two digits?)

Sorry if these questions are abit basic, but I've only been out of school for 4 months. Are direction to some documentation on this topic would help!!

Thanks guys.

 

[swertel]

I believe the part numbering philosophy dates back to the original CM controlling document MIL-STD-973. I haven't read that one fully to know for sure. But it also ties into the old drafting standards of not only ANSI, but also MIL and DOD standards.

MIL-STD-973 has been cancelled and replaced with ANSI/EIA-649 and is known as CMII. We're actually looking at redoing our part numbering/config management to match the new standard because the old one is quite costly if the FFF change is low on the drawing tree.

As far as the numbering philosophy, you are correct. Odd numbers only. The following even number is for opposite hand parts. You can use as many dash numbers as required.

--Scott

For some pleasure reading, try FAQ731-376