Every PCB Decal must have a corresponding Part Type that calls out that decal on the PCB Decals tab. Decals not called out in a Part Type will not come into the board correctly.
Please see this Tech Note for more information:
OK thanks. I understand how to assign a decal to a part in the library.
I dont think I worded my question very well but I was basically asking when you assign a decal at schematic level why pads layout couldnt find the parts/decals the netlist was asking for?
I have since got round the problem but assigning a dummy decal with same number of pins as defined by the parts data and saved in parts library.
Then when you assign a decal to the part in the schematic design - pads layout can now find the parts/decals the netlist is asking for.
So basically you cant assign a decal in the schematic if the part has no associated decal in the libray - unless you assign a dummy placeholder decal to it first.
I met the same problem， i found that assign a decal by part properties does not work. i want to know if you have solve the problem. could you do me a favor? thx.
I'm assuming you are talking about getting a part from Logic to Layout.
The part needs to be in a library. If you edit the part in Logic, you then need to save the part back to the library before you ECO to Layout. Be careful that if you changed any attributes on the part, you are going to update the attributes in the library when you do this. IMO, it is much safer to edit the library directly and then update Logic.
Check your library sort order. If you have a part defined in mutliple libraries (it is easy to accidently do this when saving) then PADS is going to use the one from the library closest to the top of the list (the first one it finds). If you changed another copy, the ECO process will never see the changes.
My English is limited, so maybe i didn't express myself very clearly. The part is in a library and it has many PCB decals. For example, RES is a part in a library and it has multiple PCB decals, such as 0805, 0603, 0402, i assigned 0603 as RES's PCB decal, using part properties in Logic. When i ECO to Layout, PCB decal change to 0805 (0805 has a high priority level). I don't know why.
There is another problem. there is a part, such as RES. It in in a library and has two PCB decals (0805 and 0603). There are two RES in schematic diagram and i want one's PCB decal is 0805, another is 0603, how can i achieve it ?
I am not sure that you are cottoning onto my sentence.
thank you for your answer.
PADS isn't very friendly about this much variation on a part. Instead of one res component I keep a generic library with a R0402 and a R0603 and a R0805, etc. I minimize the multiple decals; I might use them to have multiple anode marking options for diodes. In my mind the schematic designer needs to know the size of the part they want placed on the PCB; power dissipation is the main reason.
<right-click>(Properties) and then press the 'PCB Decals' button - Assign 0603
<right-click>(Properties) and then press the 'PCB Decals' button - Assign 0805
This might ECO to Layout without further interaction. If not:
<right-click>(Properties) and set the decal to 0603
<right-click>(Properties) and set the decal to 0805
PADS will keep the decal info in the design files. When you 'update from library' you may need to repeat these steps.
Note that there are some potential problems related to multiple choice Part types (EG part type "RES" with several optional footprints "0805, 0603 and 0402").
1) Assume you are currently working on a project with RES included and lots of 0805 and 0603 parts. If the engineer wants to add to the part type RES another footprint 1206, you could be in trouble. When you add 1206 to the part type in the library everything is good, but when you bring the updated part type into the current Pads Layout problems begin. ECO changes EVERY instance of RES (no matter what footprint is currently in the design) to the FIRST footprint in the list of available footprints. At the same time it will likely rotate the part, screwing up the routing unless you have been VERY careful to create ALL the available RES footprints with the SAME Zero orientation.
2) It may be difficult to pass the layout to 3D mechanical cad like Solidworks or ProEngineer. Check to see if the part type or the footprint is used by 3D cad. The multiple footprint are a problem if only part type is passed.
Recommendation: Have 1:1 relation between part type and footprint.