6.2 -> 6.5 BOM.ulp changes

James Littlefield wrote:

Just trying to finish up my first design done in 6.5.  When I run bom.ulp

I

no longer see the option to load a database (TSV) file.   Is there a way

to use a previously created TSV file to initialize the attributes of all

the parts and then run bom_with_attributes.ulp to get the previously

defines information.

 

I'm really not wanting to have to manually re-enter all the information

from all my *.tsv files for all each legacy design.

 

Thanks

Jim

 

I keep version 5 around for old projects, and on those occasions where I

migrate one to version 6 but don't want to mess with attributes I simply run

the old 'bom.ulp' in the version 5 ULP directory to pick up the old .tsv

files. It still seems to run fine on version 6 projects.

If there's a better way, I'd like to know also.

Bob

On 20/12/2013 12:09 p.m., James Littlefield wrote:

Just trying to finish up my first design done in 6.5.  When I run bom.ulp I

no longer see the option to load a database (TSV) file.   Is there a way to

use a previously created TSV file to initialize the attributes of all the

parts and then run bom_with_attributes.ulp to get the previously defines

information.

 

I'm really not wanting to have to manually re-enter all the information

from all my *.tsv files for all each legacy design.

 

Thanks

Jim

 

Hi Jim

I can't see anything 'off the shelf' as that would be difficult to build

for all users and their variations if it were library focused.

Initially, where would you add the attribute information. In your

libraries or as attributes attached to the parts within your schematic?

If they are personal libraries and you have been controlling them and

their names since v4 then you could target them. Otherwise I would merge

the TSV information into your schematic for each design until you get

the library parts matched with your supplier data correctly. In the v4

bom.ulp the match for part to manufacturer info was partname:value so

those combinations in your current design need to match for the TSV data

to match and enter the new attribute. If that is the approach you want

to take it would not take to much effort to knock up a ULP to do it.

This approach is similar to that used previously. Previously the TSV

data was merged with the result of the BOM.ulp output. The new way would

be to merge the TSV into the schematic, creating new attributes/values

and then run the current v6  BOM.ulp that reads attributes.

Warren

Bob...thanks for your suggestion.    I also used the old bom.ulp and it

worked fine.   Its a good stopgap measure!

Warren ..  My thought was that the information from the tsv file would be

added to attributes of the parts on the schematic.   Then you could run the

bom with attributes ULP and come up with a reasonable BOM preserving the

labor invested in the original *.tsv files.   

Perhaps I don't understand how attributes are supposed to work but my

initial impression is that they don't work that well.   As an example,  if

you have created attributes for a schematic component (say digikey part

number),  and then replace the part with a different package or change the

value,  the custom attribute (dk part number) remains at the old value.  

At least with the older method (*.tsv/bom.ulp).   Is there a good on-line

tutorial for how the attributes are supposed to be used,  how they interact

with the bom generation process, etc?

Thanks for your ideas,

Jim

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

On 21/12/2013 12:42 a.m., James Littlefield wrote:

Bob...thanks for your suggestion.    I also used the old bom.ulp and it

worked fine.   Its a good stopgap measure!

 

Warren ..  My thought was that the information from the tsv file would be

added to attributes of the parts on the schematic.   Then you could run the

bom with attributes ULP and come up with a reasonable BOM preserving the

labor invested in the original *.tsv files.

 

Perhaps I don't understand how attributes are supposed to work but my

initial impression is that they don't work that well.   As an example,  if

you have created attributes for a schematic component (say digikey part

number),  and then replace the part with a different package or change the

value,  the custom attribute (dk part number) remains at the old value.

At least with the older method (*.tsv/bom.ulp).   Is there a good on-line

tutorial for how the attributes are supposed to be used,  how they interact

with the bom generation process, etc?

 

Thanks for your ideas,

Jim

 

 

 

Hi Jim

Reading the HELP > attribute  is a good start.

Then supplement that by reading the explanations in the manual found in

the docs folder of  your installation files.

Then practice what you read.

In essence,

1. Attributes created in the library reveal themselves in the  lib, sch

and brd.

2. Attributes created in the sch reveal themselves in the sch and brd

3. Attributes created in the brd only pertain to the board

4. Then there the global attributes for the board

5. and separately, the global attributes for the schematic

To have part numbers that automatically change when you change the

package or technology, you will need to set up the attributes in the

library by device variant.

HTH

Warren

Hi Warren,

Thanks for the RTFM!  I had already perused those resources.   I think I

was not sufficiently clear in my earlier message.   My complaints with the

new attribute based bom handling are..

1.  If I have 15 2.2K resistors,  go into the schematic and add attributes

for price, Dk part number,  etc   the attributes are added to only one of

the parts.    With the old system I could have the bom sorted by component

value,  create some custom columns in the tsv file, add the information

once, and have it apply to all the components of the same value, footprint.

The only way I can see to work around this in the newer method is to have

to create a custom library for every project,  copy all the components used

in that project into the custom library, and then add the attributes in the

custom lib.  

2.  I was not meaning to imply that if I change a resistor package that the

new part would somehow magically have the correct attributes (other than

footprint).... but I could expect that it NOT have the attributes of the

part that was previously there which is what happens in 6.2.    In the old

bom handling method,   if I replace a 10K, 0805 with a 10K 0402, load the

tsv/database file  I will see nothing for the 0402 (unless it was already

in the tsv file).   This makes sense to me and when I find components in

the bom listing that have no Dk part number/cost/or other custom

information  I know to add it.

Cheers,

Jim

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

On 22/12/2013 3:49 a.m., James Littlefield wrote:

Hi Warren,

 

Thanks for the RTFM!

You're welcome, I have a whole heap of them to give out at Christmas.

   I had already perused those resources.   I think I

was not sufficiently clear in my earlier message.   My complaints with the

new attribute based bom handling are..

 

1.  If I have 15 2.2K resistors,  go into the schematic and add attributes

for price, Dk part number,  etc   the attributes are added to only one of

the parts.

Correct, adding an attribute in the schematic gives the selected named

part the attribute, not the device type.

  With the old system I could have the bom sorted by component

value,  create some custom columns in the tsv file, add the information

once, and have it apply to all the components of the same value, footprint.

Yes, the information is being added to the output of the ULP. That is

akin to adding it at a later date in a spreadsheet. The eagle design is

not being affected.

  The only way I can see to work around this in the newer method is to have

to create a custom library for every project,  copy all the components used

in that project into the custom library, and then add the attributes in the

custom lib.

Even if you have a single well maintained personal library folder from

which all your projects are drawn, it would be hell to maintain all the

part numbers for all resistor values in all package types. There have

been earlier discussions that attributes are not a desirable method of

referencing supplier part numbers. Going forward, a BOM/database

solution is needed.

 

2.  I was not meaning to imply that if I change a resistor package that the

new part would somehow magically have the correct attributes (other than

footprint).... but I could expect that it NOT have the attributes of the

part that was previously there which is what happens in 6.2.

The attributes that are there pertain to the named part on the

schematic, not the part in a library context(as said earlier). Any

attributes that were established in the library do change with the

arrival of a different part.

     In the old

bom handling method,   if I replace a 10K, 0805 with a 10K 0402, load the

tsv/database file  I will see nothing for the 0402 (unless it was already

in the tsv file).   This makes sense to me and when I find components in

the bom listing that have no Dk part number/cost/or other custom

information  I know to add it.

I like this method. It's simple.

Cheers,

Jim

 

First thoughts of modifying the ulp to import a TSV file and apply the

values as attributes runs into the problem you mentioned. If you change

the part, the attribute remains the same unless you run the BOM again

and import the TSV again. But if the TSV does not address the new part

name then it may retain the old erroneous part information unless all

fields for a given attribute are cleared initially.

So we are back to the old ULP, which works in v6.

Have you seen http://www.cadsoftusa.com/downloads/file/bom-ex156.zip

This effort by Bob Starr maybe of interest to you as it builds on your

preferred approach, uses attributes and extends to ordering automation.

All the best

Warren