Stats

  • Locked Locked
  • Replies 13
  • Subscribers 165
  • Views 27895
  • Members are here 0
More Content
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

OrCAD Capture 16.5 Allegro Netlist Fails (ORCAP-36003)

RalphGibson

Hello all,

I'm running OrCAD 16.5 and am having a problem generating an Allegro netlist.  Creating a Tango or ComputerVision format netlist works fine. The Allegro netlist operation fails with the following messages for all simple parts:

#1 ERROR(ORCAP-36003): Conflicting values of following Component Definition properties found on C10 and C1 for part "CAP_SMT".
PCB Footprint
VALUE

C1 gives this error for C2 through C11.

3 180-REG-001644  CAP_SMT  4.7uF  CC1210  10%  16V  C1,C6,C7
8 180-REG-001618  CAP_SMT  0.1uF  CC0402  10%  16V  C2,C3,C4,C5,C8,C9,C10,C11

I've been using OrCAD since about 1987, so am fairly comfortable with the product.  However, I haven't tried to generate an Allegro netlist for several years.

I'd appreciate any pointers as to what is causing this error, and if there is a solution I can implement.

I'd prefer not to delete all of the properties I've added, as they help with the BOM generation in Excel.

Thanks in advance for any recommendations.

Cheers,

Ralph

  • RalphGibson

    Hello Oldmouldy,

    Sorry for the delay, but unfortunately I can't seem to attach a file to this message.  When I click the "Insert/Edit Media" icon, I get a blank space with only a close box icon showing, with no way that I can see to select a file to attach.  I've also tried using my mouse to copy/paste with no luck.

    I see the same problem with Chrome and Internet Explorer, and from my work or home PC.

    Do you know of any other way I may be able to attach the file to get it to you for review?

    Or do I need to request "file attach permissions" or some such from Cadence?

    Thanks for your help with this.

    Cheers,

    Ralph

  • oldmouldy
    Looks like this might be broken, I will see if I can get a request in to fix this.
  • RalphGibson

    Hello Oldmouldy,

    I believe I have a way to get my OrCAD design ZIP file to you.  I have a personal hobby website at www.gibsonsjewelry.com, and have attached the zip file to an animated GIF icon in the upper right corner of my tools page.  The icon is a cartoon character banging his head on his computer keyboard.  If you click on that icon you should be able to save the archive .zip file.

    Please let me know if this works for you, and thanks again for you help.

    Cheers,

    Ralph

  • oldmouldy
    Hi Ralph, well, that worked! The issue is that you have a Property Named "Device" attached to the parts and the "Device" property Value is the same for parts with differing properties, the "Device" is supposed to be an identity for "this part" and therefore the properties cannot differ. If you remove the Device Property, looks like this is a property on the library part so you will need to remove it from the library part and update the Design Cache, the Capture / PCB Editor netlister will build the Device Property value from other property values attached to the parts in the schematic.
  • RalphGibson

    Hello Oldmouldy,

    Thanks very much for downloading and checking the design file for me and locating my problem.  Much appreciated.

    I checked the part properties for a design from another engineer that doesn't have this problem, and sure enough there are no "Device" properties in those part symbols.

    It appears the "Device" property has a very specific meaning in the Allegro layout tool that I wasn't aware of.  Since I have used the Tango netlist generated by OrCAD Capture for several years, this never came up.

    The only reason I added the "Device" property to each symbol is to improve sorting and grouping parts when generating a BOM.  So I'm not overly attached to that specific name.  Could I simply update the properties in all of my symbols to change "Device" to "Family" or something similar?

    Also, is there a list of device fields or properties for the Allegro tool that have specific meanings that I should avoid?

    Thanks again for your help with this.

    Cheers,

    Ralph

Cadence Guidelines

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.