Stats

  • Replies 7
  • Subscribers 161
  • Views 14389
  • Members are here 0
More Content

New to PCB Editor and some questions

stellar

 I've used Layout for many years and this week started my first board in PCB Editor. I haven't taken a class and have stumbled along with a book I bought on Amazon so help.

First off the colors don't work correctly for me. I cannot get the bottom pads to appear red and the top pads to appear blue. I've turned off every color and brought up just the top and bottom pad colors to try and get it correct. I can get the top and bottom silkscreen to agree with the chosen color but not the pads. I did find that using hollow pads does at least give me the chosen color for the outline of the pad which is good enough for now but I sure would like to see colors that match the selected color. Another strange thing is the pads on the parts when filled is selected can take on various colors on both the top and bottom layers. It seems messing around with the color selections cause this and there is no way to undo it.

I'm using the symbols for capacitors and resistors that come with Editor. I find that I can move these symbols on top of another part that has a place outline and no DRC results. I only see DRC's when the pads of these parts overlap the pad of another part. Perhaps these library parts weren't create with place outlines or I need to turn something on to get place outline DRC errors. 

When highlight is turned on in Editor I properly see the part selected highlight over in Capture but I cannot move the part in Editor. In Layout I could cross probe and move parts at the same time.  I would like to be able to select and move a part in Editor and have the part and associated page in Capture follow the selection.

One thing I miss from Layout is hitting the C key to center the view. With Editor I feel like I'm having to use the mouse wheel a lot to reposition and place parts. Are there any hotkeys that can make centering easier? 

 When I select a symbol in Capture it highlights properly in Editor but the display zooms in and fills with that part. If the part is an 0402 resistor the part fills the display. I would like no zoom only highlite so I can survey the location and zoom when I want to after the selection. This must be a setting somewhere. 

 

 

 

 

 

 

 

 

  •  Hi stellar,

     First off, I believe this post belongs in the PCB Design forum since that covers general aspects of the PCB Design tools, including Allegro (PCB Editor). This forum is for SKILL, which is a languge you can use to extend the base functionality of Allegro.

    With that out of the way - Welcome to Allegro! I think it's a huge upgrade over Layout, especially since v16.0, and hopefully you'll appreciate all the power of Allegro and put it to good use!

    I will number your questions for clarity:

    1a.  The pad color is controlled by the Pin column in the Stack-Up > Conductor folder of the Color Dialog form (Display > Color/Visibility). If you change the color swatch in the Pin column, you should see the pad color change. This will be reflected in the Pin column of the Visibility tab of the Control Panel (on the right side of the PCB canvas).

    1b. Taking on "various" colors seems a bit strange. I don't quite know what you mean. Can you clarify? What are you doing and what is happening?

    2. I suspect the symbols don't have a PLACE_BOUND shape. If a PLACE_BOUND_TOP shape collides with another PLACE_BOUND_TOP shape, you will get a DRC error. Check that the symbols have this shape. If not, that explains why no DRC errors are created until the pads touch.

    3.  I don't believe this is possible - picking up a component doesn't highlight and cross-probe the component. But you can move a highlighted and cross-probed component.

    What app mode are you in? Using Etch Edit with Symbols turned on in the Find Filter, you can pick Highlight from the RMB menu and then click on the symbol to move it. Not much added work.

    4. Could View > Zoom Center be what you're looking for? If so, you could make Zoom Center a funckey and then you'd just have to hit a single key and click the LMB to center on the cursor click. Not quite as convenient as what you're asking, but perhaps good enough.

    You might also explore using Strokes (Tools > Utilities > Stroke Editor) which can be quite powerful and same considerable time.

    Conversely, I find the current behavior great because I can zoom in with the mouse wheel, do some work, scroll out with the mouse wheel, move the cursor, zoom in to a different point with the mouse wheel, etc. Different strokes...

    5. Indeed there is. Check the no_zoom_to_object Preference in the Ui > Zoom folder of the User Preferences Editor form at Setup > User Preferences.

  • 2. I suspect the symbols don't have a PLACE_BOUND shape. If a PLACE_BOUND_TOP shape collides with another PLACE_BOUND_TOP shape, you will get a DRC error. Check that the symbols have this shape. If not, that explains why no DRC errors are created until the pads touch.

    You should also check these layers, both the PLACE_BOUND_xxx and DRC are turned on (menu Display->Color) and Select Stack-up Non-Conductor for DRC and Package Geo for place bounds.

    4. One thing I miss from Layout is hitting the C key to center the view. With Editor I feel like I'm having to use the mouse wheel a lot to reposition and place parts. Are there any hotkeys that can make centering easier? 

    The following assignement added to your local env file will do this:  funckey c "zoom center; pic -cursor"

    If you want a capital "C" then just substitute the C for the "c".

  • Hi

    One small note, there's a small spelling error in the answer, to get c to zoom center the command is

    funckey c "zoom center; pick -cursor"

    pick missed the k :-)

    Best regards

    Ole

  • Your pins not matching the color you've set could be related to the OpenGL settings inside PCB Editor. The Pads and traces will look transparent which can sometimes be described as different. These settings enable you to view through all the layers of the PCB. If you don't like this the go to Display - Color Visibility - Display folder and change the global transparency to 100%. You can do the same for shapes if you want to. This should display the colors as you are expecting.

  • Okay had the DRC color turned off and all the parts in question did have the place boundery top so all is well there.

    Please elaborate on the local env file. Is this a text file someplace where you can enter funckey definition strings?  

     

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.