OrCAD Capture ---> PCAD ?

[SphinX]

orcad land

Salam,

Ok i designed many of projects using OrCAD .
OrCAD Capture is vell good but Layout.

So I decided to draw my design in Capture then export the netlist file to PCAD to design the layout.

How can i do that ?

Thanks

 

[alex840]

export concept to pcad

at first i will comment concept of pcad's attributes "type" and "pattern". "Type" - it is component description, which contains mapping between pin numbers of the component and the land pattern. "Pattern" is graphical description of land pattern. originally, orcad has only "PCB footprint" attribute, and, if you plan to use special land pattern for each type of component("Type"="Pattern"), it is enough to transer only "PCB value" attribute. after this, you will get component of "type" C0805 and "pattern" C0805. it is not so convenient and i prefer to use additional attribute in orcad, to share the same land pattern among components. but in general it will be enough to use ony one attribute.

so, you will need to transer three attributes from OrCad to Pcad:
1. part value (it's quite obvious, orcad has this field)
2. some attribute, which is called "Type" inside Pcad. make additional attribute, for example, make new column "Type" by Property Editor.
3. land pattern name. you can use "PCB value" attribute, or you can make your own(Pattern, for example).

after this you should make netlist. inside orcad, use Tools->Create netlist, choose "Other" tab and choose "tango.dll" as formatter, use {Value} as Combined property string fro the part value and {PCB Footprint}\n{Type} as Combined property string for PCB footprint. Check "View ouput" checkbox and press "Ok". You will get netlist to your screen. Be carefull - Pcad doesn't like additonal lines at the top of this file, for examlpe - contens of your design/sheetname fields. Netlist should start like this:

[
C1
0603
C0603
100pF
...

after this, you can load netlist to Pcad by "Utils"->"Load Netlist" inside PCAD PCB. But at first you need to draw land patterns by Pattern Editor and to make corresponding components by Library Executive. And you also need to setup your libraries by "Library"->"Setup" in PCB.

if you have additional questions - ask me.

alex

 

[bigrice911]

what is pattern in orcad

hei, man, you could use PCB navigator to do the job instead of changing the netlist manually.

PCB navigator can make From-and-To translation between: Orcad, WG, Zuken, PCAD and PADS.