Circuit Negma

C++, C, VB.NET, PCB, Electronics, Circuit Design

Archive for February, 2010

MentorGraphics PADS Layout :: How to extract an IPC-356 netlist from PADS

Posted by Circuit Negma on February 8, 2010


Created By: Hussein Nosair

Symptoms
    How to extract an IPC netlist from PADS Layout
    How to output an IPC356 netlist from PADS
    How to extract an IPC-356 netlist

 

Solution:

PADS 9.0 and newer:
Beginning with PADS 9.0 there is native IPC netlist extract capability.  Go to File > Export and change the "Files of Type" from ASCII Files (*.asc) to IPC 356 Files (*.ipc).  After clicking save you will be able to choose between IPC-D-356 or IPC-D-356A netlist output.
PADS2007.4 and older:
The older versions of PADS do not have native IPC netlist extraction.  However, you can download a VB script that has been written by a 3rd party vendor at CapeCAD.com (note, the VB script has not been tested by Mentor Graphics and we assume no responsibility for it’s accuracy).

Posted in PCB | 1 Comment »

MentorGraphics PADS Logic/PADS Layout :: How to create a part with alphanumeric pins?

Posted by Circuit Negma on February 8, 2010


Created By: Hussein Nosair

Symptoms
    How to create a part with alphanumeric pins?

 

Solution:
  1. Create your PCB decal as usual (you might use the Wizard), assign the alphanumerics (you can use the Tools > Assign JDEC Pinning to expedite the process). 
  2. When done go to File > Save Decal. Be sure that the check mark for Save Alphanumerics is checked.
  3. Type in the correct part type name in the box provided and click Save.
  4. Go back to PADS Logic and edit the Part Type.
  5. Create your CAE decal as usual (you might use the Symbol Wizard), add the pins, but do not assign pin numbers. Save the CAE decal.
  6. Edit the Part Type that you created.
  7. Select the Alphanumerics tab and confirm that the alphanumeric assignments match up with the PCB footprint pin numbering (Pin 1 = A1, Pin 2 = A2, etc).
  8. Select the Gates tab and add all the necessary gates and assign the corresponding CAE decals.
  9. Select the first Gate and look at the lower portion of the dialog window.
  10. You should see a series of alphanumeric pin names listed under the Unused Pins column (if not, you should select all the pins on the right hand side for each of the Gates and press the Remove button).
  11. Add each alphanumeric pin in sequence so that the CAE decal will have the pins in the correct order (you may want to edit the CAE decal again to confirm how the sequence numbers appear on your decal. Sequence numbers appear on the pins as #1, #2, etc). You will see the listing of sequence numbers in the Gates tab as well as you add each pin to the gate.
  12. Continue adding pins for each of the gates.
  13. Go to the PCB Decals tab and assign the PCB footprint for this part and then click OK, then save and exit from the Part Editor.

Note:  The sequence number maps to where the alphanumeric pin shows on a CAE decal, but the Alphanumerics tab maps how the alphanumeric pin will relate the the PCB footprint pin assignments.  It is much easier to build the part in reverse as described above because the JDEC pinning in the PADS Layout Decal Editor will speed up the alphanumeric pin assignment process.  Assigning the alphanumerics as you go in the CAE symbol can result in incorrect PCB footprints later down the line.

Posted in PCB | Leave a Comment »

MentorGraphics PADS :: PADS Layout: PCB footprints are not correct when forward annotating from Designer

Posted by Circuit Negma on February 8, 2010


Created By: Hussein Nosair

Symptoms
    PCB footprints are not correct when forward annotating from Designer
    PCB decals are wrong when updating design from schematic

 

Solution:

In PADS Layout go to Tools > DX Designer and select the Preferences tab.
Place a check mark in the box for "Compare Part Decals".
With this box checked the comparison between the schematic and PCB design will look at the PCB footprints assigned and update any applicable parts in the design.

Posted in PCB | Leave a Comment »

MentorGraphics PADS :: The wrong part type or decal is selected when importing netlist

Posted by Circuit Negma on February 8, 2010


Created By: Hussein Nosair

Symptoms
    The wrong part type or decal is selected when importing netlist
Solution:

The order of your library list is very important in this matter. You may have multiple part types and/or decals with the same name in different libraries. Confirm that the correct library is at the top of the Library List. PADS Layout will use the first Part Type or Decal it finds in the list. To change the order go to File> Libray> Lib List, select the libray and click the Up button until it is at the top of the list.

Posted in PCB | Leave a Comment »