Stats

  • Locked Locked
  • Replies 5
  • Subscribers 167
  • Views 22241
  • 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

DRC errors: package to place keepout spacing

Jengle

Who can tell me how to solve it ?

Thank you very mach!

  • EvanShultz

     Hi Jengle,

     It sounds like you have a place keepout area, and there is a footprint inside the place keepout. Apparently you've found the DRC error itself, and the issue is where you see the bowtie. You should be able to see the problem if you can find the bowtie.

     If you can't locate the issue on the PCB, use the Display > Status form. Click on the colored box (in your case, either red or yellow) by "DRC errors" in the DRCs section of the form. This will bring up a report of DRC errors. You can click on the coordinates in the reportto jump to the issue.

    If you've already at this point, and you can't figure out what's going on, we need more information to help you. Post a screenshot of the problem. Make sure all subclasses are turned on (Display > Color/Visibility) because the issue could be on a subclass that is turned off, which would make the issue tough to see.

  • Lowee
    Hello everybody,

    I've got the same problem with DRC errors... (It's good to know that I'm a new user of Cadence Allegro)

    So, first, I created the symbol of my PCB with route & package keepout (package keepout has constraint with package_height_max because of my PCB will be implement in an aluminium box). After setting those parameters, I create the board project including the drawing of my PCB (*.dra).

    Then I import the logic netlist (exported with Allegro Design Entry CIS) and when I place every connectors and components, a DRC error is appearing...

    You might found a screenshot of one of this problem.

    I'm using Cadence Allegro 16.3 on ASUS X53 Series Windows 7

    I hope someone can help me to fix it up... Feel free to ask me some questions if I'm not clear with these explanations.
  • Lowee

     Hello,

     The problem was fixed, the solution is to set the constraint of package keep out with package_height_min and not package_height_max. With constraint package_height_max, DRC will be automatically generated.

     

    Hope it can help some people.

  • shatwood

     Hi!

     

    I have the same problem on a current design, where did you change the constraint values?

    can't find it on constraint manager.

     

     

    regards, Julian

     

     

    I was now able to solve the problem, 

     

    i changed the "package_height_min" of the "keepout_top" layer to the actual height of my symbol,

    and then changed the "package_height_max" of the "place_bound_top" layer of the symbol to symbol's actual height. 

    Now, there is no conflict anymore.

    contact me if you have further questions

     

    Regards,

     

  • Lowee

     Hi Julian,

     You have to change properties of shape that you create on your design (if you create it).

    1) Select shape with PACKAGE_HEIGHT (min or max) constraint

    2) Then right click on shape and select "Property Edit"

    3) In Property Edit pop up window, select PACKAGE_HEIGHT_MIN and set the maximum height to place your components

    4) Option: if you not sure, you might RESET or DELETE properties you set.

     

    This is like in your house (YOUR BOARD), the PACKAGE_HEIGHT_MIN might be 2.10 meters, if a friend (COMPONENT) come to your house (he tall 2.15 meters) he can't come in...

     

    Hope it can help you !

    Warmly,

     

    Louis

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.