[HELP] Orc@d "PCB footprint" property

[maestor]

resistor pcb footprints

Hi guys,

I am a newbie with Orc@d :roll: and I was wondering how you normally set the "PCB Footprint" property.

1) When a place a component in Capture from the libraries the PCB footprint is empty, is that right?

2) Is there a way to just add the component from the library with the PCB footprint set

3) Is the UPD file the fastest/best way to update the PCB footprint property?

4) Is there a list of PCB footprints' notation supported by Orc@d somewhere?

Thx all in advance

-maestor

 

[fastelec]

property pcb footprint

With "PCB Footprint" property in Orcad you can set a footprint for a given component.Yes it`s right when you place a component this property is empty.You must to set it manually or automaticly when using a macros.You can view footprints in Orcad layout.For example i filled the PCB Footprint in my design for resistor with "SM/R_0805" witch means than i linked a R_0805 footprint (it`s a smt pad ) to a the element from the SM library.IN "Orcad layout" all footprint can be viewed when you click in tools menu "library manager" (this is for orcad 9.2).

 

[falling_stone]

capture pcb footprint property

Hi, Maestor.
You may add PCB footprit at any time You like before You produce a netlist.
So,
1 - Yes, and when You will try to produce a netlist Orc@d will not allow You to do that untill You fill up all of the PCB footprit properties (I'm not sure this is true for all of the netlist formats)
2 - In order to do that You just have to open component for editing (within a library, not a local copy) and than double click on the free drawing space to open Part Properties dialog. Find there existing PCB footprit property of create it Yourself, fill it, than save the part. From now on each time You will add this part to Your designs You will have this property set. (By the way, if You already have this part in Your design dont forget to update its local copy, step on the part name in the Design Cache section in design hierarchy window and run Update Cache command on it (this command is present at either local mouse menu or somewhere in menu bar, sorry, I dont have Orc@d near me now, so please check help for it)).
3 - If You want to update big part of Your design the UPD file is a really helpfull thing, as an alternative way I may suggest using spreadsheet editor with multiple components selection. (The spreadsheet editor is written in a strange way, there Ctrl-C/V and Ctrl/Shift-Insert is not the same, try also different selection type (as a whole or inside the text), just try it.) You may select different components either directly in the schematic page and then press Ctrl-E to edit their properties or use Browse Parts command, select multiple components in the table there (You may sort them there according to their properties listed in column names) after You have done with selection - press Ctrl-E.
4 - I did not understand this question, but if You mean a list of the footprints alredy existing in Orc@d Layout I think You may find it in user manual, If You mean a template for the new PCB footprint name creation, You may just use any name You want, there is no prefference from software point of view, just be sure that it correspond to the name of the component in layout library.
Best Wishes,
F.S.

 

[maestor]

Hi,

Excellent answers
I have started editing parts (within the library), things like resistors, caps...and it works fine.

About the UPD, sounds quite straight forward using the spreadsheet editor. One thing that comes to my mind is that the UPD files look a quite powerful thing, you can update properties of your design in a very fast way and some parts are common to a lot of designs, resistors, caps, regulators, connectors...so why people don't share them? I had a look in google and I couldn't find UPD files at all.

About question 4, yes I mean a list of the footprints alredy existing in Orc@d Layout I guess as "fastelec" said it can be accessed in -> tools menu "library manager".

Thx guys,
-Maestor