[SOLVED] Cadstar - partnumber visible in PCB layout?

Hi all,

Is there a way in Cadstar to make the partnumber that is associated with a part in the library, visible in the PCB layout? As far as I can see, the only things you can make visible in the PCB layout are either the component reference or the part name.

Maybe it is possible to attach an attribute to the PCB component that will call out the partnumber when the part is added to a PCB layout?

thanks!
Waljit

- - - Updated - - -

Another way of asking this same question is, how do I access the built-in cadstar attributes for partnumber (or part description) for a PCB component in a PCB layout?

e.g. in a library you might have:

.cadstar_part_name (my_part_number) ;my_part_description
pcb_component_name
*DFN cadstar_part_name
etc... etc...

How do I access the fields my_part_number and/or my_part_description [that are already defined in the library] for a part or component that already exists in a PCB layout?

Waljit

In the part library you make an attribute name, the usage needs to be symbol (to be seen in scm only) symbol and component (to see in both scm & pcb) or type component (to only see in pcb).

This attribute needs the same usage in ALL parts libraries.

In your scm/pcb you can then edit this attribute in the attribute editor (unless you make it read only on the definition last tab) and display it by enabling it in the colours setup.

On the pcb, in the defaults\text tab there is an attribute setting that puts them on the silkscreen (or your chosen layer) when you bring in a component that does not have them controlled by an origin.

If you want to see the part number in scm/pcb then you need to duplicate the part number attribute (visible in the item properties of attribute editor etc) as a user attribute.

Hi Mattylad

Thanks for the quick reply. Yeah, I know how to do it by adding an extra attribute into the library.

But, the part number I want already exists in the part definition in the library - in brackets after the partname. What I would like to do is to make that information available from within the schematic or pcb, *without* having to do further edits to the library. Is this possible?

I've tried playing around with several ideas, but none of them worked, so I think the answer might be a "no".

thanks
Waljit

No it is not possible.
I suspect that its something that was not considered when it was introduced and has not been added as an option given the very easy way of replicating it.

Use a duplicate in a user attribute.

Its the only way, its easy to do, simply create the attribute name, select the entire number column in the library and copy/paste to the new one.

BTW - you mention its in brackets - that sounds like your using notepad - use the library editor instead.

OK, thanks for the reply. This will be quite a change, as we have multiple parts sharing the same definition ((
This will have to be changed to 1 part for 1 definition, before the extra attribute can be added.

Also noted your point about using the GUI rather than manually editing the lib files. Old habits die hard ;-)

thanks
Waljit

I would say that to have multiple parts using the same definition now is going to cause problems.

With the introduction of attributes it is essential that the definitions are unique and relate to single parts only.
Copy the part name to the definition name-that way they match, can be easily found etc.
It might take some time to rework the parts & definitions but then you should be able to reload them quickly using the Actions\Replace/reload dialogue.

Using unique definitions will however open up a new world of useful attributes that can be used to save more info with the part such as:
datasheet hyperlink, manufactures & suppliers names and order codes, Value, wattage, voltage, package, company order no, FEC/RS numbers etc.
The more you put in the more you can get out.

My habit of using notepad died several years ago, the libed used to be awful - but the Library Editor now is excellent and I will only use notepad to open a corrupted library file (which is very rare).

BTW - using the library editor in V13+ means you can copy/paste parts including the definition to enable easy duplicating of parts and just changing the part/definition name.

Notepad rules....
You can separate multiple parts quickly by using cut and paste in note pad to put the basic parts info under each parts name. You do not need to add the *DFN line, this will be automatically added when you read the parts library into lib manager for final tidying up.

Thanks all. For all new parts from now on, we'll use the GUI with one part per definition.

Whilst I am here, what's the recommended method for dealing with non fitted components in the BOM? I tried the variant manager, and it works, but it seems a bit overkill if you don't actually have more than 1 board variant. Is there an easier way? You could use an attribute, but then we're back to the same library problem as above ((

Id go for the variant manager option myself, the amount of things that variants enables like printing schematics that do not show not fitteds, separate boms etc make the extra work worth it.

However if you want the attribute path then you you need an attribute per part.
make it symbol & component usage so it can be edited in the design.

You cannot call it "fitted" as that name is reserved so call it "is_fitted" or just "fit" and make the default value 1. This can be applied to all parts in the library within seconds with copy, select column and paste.
Reload parts then use the attribute editor (although you can just make the attribute in individual designs rather than in the library).

If its called "is_fitted" and the default value is 1 then in the report generator do a condition check like.
IF is_fitted =1 (components)
component name
part name
and so on
next.

That way it checks for the value being 1 and the outputs the bom if true.

in your variant you simply change it to 0 or remove the value (or use YES/NO).
You can make multiple variants using attributes by having an attribute per variant.
I.E V1_Fit, V2_fit and so on.

You can even get clever with attributes and even put part numbers in them so you can change parts with different reports - but thats getting a bit complicated.

Not as good as true variants but a poor mans version.

Thanks for this Mattylad.

One more question about variants - is it possible to display the variant name on the schematic itself? That way, when the scm is printed, you can see which variant has been printed. If not, can this be raised as an enhancement request? (along with being able to display the part number field in the PCB layout, the usage case for this being e.g. for assembly drawings).

cheers
Waljit

- - - Updated - - -

Ignore the last post - found it (not sure why I didn't find it when looking last night!)

The "add design field" in a text box gives me what I need.

if you have variant manager use it, it does what it says and it works, far better than using attributes and writing special reports, and in the end the time you save by using variant manager pays for its self in less problems...

Thanks Marce.

One last, final question on this topic (honest!); what is the recommended way to add items to the schematic that you want to appear on the BOM (such as jumpers, mating halves for connectors, the bare PCB itself, etc...) but they have no connectivity or nothing electrical associated with them? Up to now, I add them as parts but with a special "NULL" PCB component which has no pins, pads or copper. Seems to work OK. Is there a better way?

And, is there a way to get the parts list output and/or report generator to stop things like mounting holes from appearing in the BOM? [I guess they come out in the BOM because they are setup as parts. I looked for an "exclusions" option, but didn't see one anywhere].

OK, that was 2 questions ;-)

Cheers

You can put your mounting holes on a separate sheet, "non bom items" so you can have holes, fiducials, tabs, etc on that and just do not select that sheet when doing the BOM.
then you can also put pcb stuff like heatsinks etc that do want to be on the BOM on yet another sheet.
This way they are not printed out with the schematic but still available for ECO update etc.

Or for the report generator if your not able to select the sheets, add something to the parts and excludes them form the report.
Look at the placement.rgf that comes with CADSTAR for examples of this, it has some IF <> Mech type lines.
Again - an attribute can do this, when the part is created it can have a default vale given so that standard reports can exclude it.

The null component for a part is common, I often see this for the PCB itself, that way the BOM includes the board too.

Great, thanks all!