Access 2000 and CIS ORCAD misunderstanding

[pavel47]

orcad [footprint viewer type]

Hello

In my Access 2000 database I have Part Number as follows:

TRAN0001
TRAN0002
.
.
.
TRAN0022

When I configure my CIS for this database and see Database
Parts Window id CIS Explorer these Part Number values are reduced to

0001
0002
.
.
.
0022

It's annoying as I have several tables and Part Number format of each table take the form:

W_10000
W_20000
.
.
.
W_N0000

where W_1, W_2, ..., W_N are sets of caracters
and 0000 - four numbers.

When I try to update components after linking, it appears that some components are the same Part Numbers.

What can I change to correctly transfer Part Numbers in CIS?

Thanks.

Pavel.

P.S. In my database I set format of Part Number to be Text.
First I tries with Autonumber, but it seems that this format is incompatible with CIS.

 

[albug]

Re: Access and CIS ORCAD configuration

I don't think your part numbers are being reduced. I think you probably also have an ID field in the database and this is being shown in CIS Explorer and confusing you.

Your Access database should have a "ID" field and it is best if this is set to "Autonumber" for the type. This will help to keep unique ID's for each record. Set this "ID" field as the Primary Key in the table. The CIS configuration wizard will display this field as "Counter" and will not have any problems with it.

Keep your existing "Part Number" field in the database (ie. W_N0000) in the various tables. In the CIS Configuration Wizard, for each table in your database, set the "Property Type" for this "Part Number" field to "Part_Number" and check the "Transfer to Design" box.

Now, to see the Orcad layout footprints in CIS explorer ("PCB Footprint" field), exit Capture CIS then:
1) Open "Capture.ini" in your CIS program folder (ie. C:\Cadence\PSD_14.2\tools\capture)

2) Look for the section labeled as "[Footprint Viewer Type]" and set the "Type" line below it to:
"Type=Layout"

3) Look for the section labeled as "[Layout Footprints]" and create "DirX" entries below it pointing to your footprint library paths. For example:
Dir0=C:\Cadence\PSD_14.2\tools\Layout_Plus\Library
Dir1=C:\Data\Cadence\Libraries\SFM\Main\Footprints
Note: Capture CIS will automatically look for PCB Footprints in all libraries located in the above directories.

Finally, to be able to see the schematic symbols in CIS Explorer, make sure you have added each symbol library to the Capture CIS search path:
1) Open a schematic page in Capture CIS
2) Hit the "P" button to place a component
3) Click "Add Library" and then add each library with symbols (referenced in your database).
4) Restart Capture CIS in order for CIS Explorer to start using the new libs