Home > Community > Forums > PCB Design > PCB Editor and "find"

Email

* Required Fields

Recipients email * (separate multiple addresses with commas)

Your name *

Your email *

Message *

Contact Us

* Required Fields
First Name *

Last Name *

Email *

Company / Institution *

Comments: *

 PCB Editor and "find" 

Last post Fri, Jul 4 2014 12:16 PM by Quarkdog1. 36 replies.
Started by TH Designs 24 Jul 2012 09:00 AM. Topic has 36 replies and 7711 views
Page 2 of 3 (37 items) < Previous 1 2 3 Next >
Sort Posts:
  • Tue, Jul 24 2012 6:57 PM

    • ScottCad
    • Top 50 Contributor
    • Joined on Sat, May 26 2012
    • Roswell, GA
    • Posts 176
    • Points 2,775
    Re: PCB Editor and "find" Reply

    Tom, Roger I did a bit more bit twiddling and found a few things. In general edit mode you can right click "Super Filter" and choose any item in that menu then turn off the superfilter and you will be able to find parts with highlight and zoom to where they are located on the board. If you then choose to do something else like change modes to etch edit then the Find part operation will not jump to the part if you are zoomed in on another area of the board. You have to be zoomed so you can see where the part might be. 

    The find part or symbol/pin operation reverts to only highlighting a part in either the world view or if you are zoomed out to see the board.

    Thats ok if your zoomed out but useless if you are zoomed in on another part of the board.

    The other option if you are zoomed in on one particular part of the board and you choose options find a symbol/pin is to use the zoom selection icon to jump to the parts location. Thats kind of useless too as who would think to do that ? and why should you really have to.

    It kind of gets worse from here. Lets assume for a sec you are working on a moderate sized board and you are in "EE" mode and you decide to route a trace from c1 that might be located somewhere else on the board. You choose options > find, enter your symbol reference C1 in the dialog box and hit enter and the UI just sits there. It does not take you to the location you requested unless you then choose to hit the icon Zoom Selection to get there. In certain circumstances you may end up either zoomed out from the part or zoomed in correctly so it is easy to route from a pin. Dont think this cuts the mustard. Honestly the mechanics of this operation of finding a part with zoom to location is not workable for anyone that would like to be productive with the editor IMHO.

    Saved the best for last.. There is more. Suppose we are zoomed in on a part of our board and we want to go to say c3 thats at the other end of the board. This time we decide to click the icon on the toolbar called "show element" we could also use the F4 key to do this. So we hit the F4 key for show element then go to find > Options and enter C3 in the dialog box. The screen will pan to the location of the part and highlight it but there is a window that pops up covering the actual part we were looking for with info about the part LOL....Hard to believe..

    Now one could argue that show element is not really a find operation as we want info about a particular element. The point is that the actual UI will pan to where that part is located which is what we were after so the begging question is why on earth it does not do that by default for any find operation at a certain Zoom level.

    I dunno, seems to me this is broke in a bad way or not very well thought out period. It's hard to be productive when you literally got to will the software to do what you think it should do for a given operation. New users will have a horrible time getting to grips with these hidden treasures. Hard to believe that find feature ever made it through QA...

    I think by way of a suggestion a better method would be to treat the find operation like this. If the object you wish to find is not in the scope of your window then the Software should know that you wish to both find the object and zoom/pan to that location and highlight the object too. That might be an ez fix. Having to invoke a "Super Filter" operation first before you then choose Find is non productive.

    Thanks Scott.

      

     

    • Post Points: 20
  • Wed, Jul 25 2012 2:44 AM

    • steve
    • Top 10 Contributor
    • Joined on Fri, Jul 18 2008
    • Woking, Surrey
    • Posts 1,162
    • Points 18,880
    Re: PCB Editor and "find" Reply

    Finding parts has three ways.

    1. Invoke a command in PCB Editor like Display Highlight or Display Assign Color then in the FInd by name type the refdes of the part you want and hit tab or return and the part is highlighted and zoomed to.

    2. No active command type the refdes in the Find by name, it is shown in the world view, then click on the Zoom to selection icon.

    For both of these to work you need to make sure that Symbols are checked in the Find Filter.

    3. No active command - left mouse button the part in the schematic and it zooms to object in the PCB.

    You can also type refdes <refdesname> hit return at the command line and the part is selected then use zoom to selection icon.

    You could also raise an enhancment request with Cadence / VAR to Improve this function..... 

    • Post Points: 35
  • Wed, Jul 25 2012 4:48 AM

    • mcatramb91
    • Top 75 Contributor
    • Joined on Thu, Jan 3 2013
    • Chelmsford, MA
    • Posts 95
    • Points 4,920
    Re: PCB Editor and "find" Reply

    Sorry for being late to the conversation about this but I have a couple things to add:

    1. As far as I can tell <Ctrl>+F isn't a standard function inside of Allegro, even in the 15.7 days, it must of been some custom SKILL code or special alias that would allow it to work.
    2. If you want to zoom/center on a component just type symbol followed by the reference designator on the Allegro command line then LMB Click inside the WorldView to zoom/center on the selection (WorldView is to the right of the Allegro command line by default)
      • You can also click on the Zoom Selection Icon to center the display as well. (Zoom Select Icon is between the Zoom Previous and Redraw icons on the toolbar)

    For example, to zoom/center on Ref Des U2 type symbol U2 on the command line to temp highlight the component and if it does not zoom/center on the component then LMB click inside the Worldview to zoom/center the display. (or click the Zoom Selection icon)

    I personally always used Show Element (Display > Element) to find components which would zoom/center the display by default.  I would start the Show Element command and type symbol or comp followed by the Ref Des.  You could even create an alias to do it quickly:

    alias find "show element ; comp"

    After this alias is set then just type find followed by the reference designator on the Allegro command line and it will zoom/center on the component. (downside the show element window will appear which you can just close.)  Also note that comp on the command line will only work with the Show Element command.

    Hope this helps,
    Mike Catrambone
    Plexus Engineering Solutions

    • Post Points: 20
  • Wed, Jul 25 2012 4:54 AM

    • fxffxf
    • Top 25 Contributor
    • Joined on Thu, Jul 17 2008
    • ., AK
    • Posts 290
    • Points 4,620
    Re: PCB Editor and "find" Reply

     You should try typing in the allegro command area: refdes c1

    • Post Points: 5
  • Wed, Jul 25 2012 5:12 AM

    • steve
    • Top 10 Contributor
    • Joined on Fri, Jul 18 2008
    • Woking, Surrey
    • Posts 1,162
    • Points 18,880
    RE: PCB Editor and "find" Reply
    This only selects the part in the world view. I still need to then click in the world view or use Zoom selection.
    • Post Points: 20
  • Wed, Jul 25 2012 5:19 AM

    • mcatramb91
    • Top 75 Contributor
    • Joined on Thu, Jan 3 2013
    • Chelmsford, MA
    • Posts 95
    • Points 4,920
    Re: RE: PCB Editor and "find" Reply

    After something is selected in the design LMB Click inside of the WorldView and Zoom Selection icon work the same way - zoom/center on the component on the design not just the WorldView

    Mike

    • Post Points: 5
  • Wed, Jul 25 2012 6:18 AM

    • TH Designs
    • Top 25 Contributor
    • Joined on Fri, Apr 13 2012
    • Warminster, PA
    • Posts 269
    • Points 4,370
    Re: PCB Editor and "find" Reply
    mcatramb91:

    As far as I can tell <Ctrl>+F isn't a standard function inside of Allegro, even in the 15.7 days.

    Mike,

    In Orcad Layout <Ctrl>+F was a standard feature. I have used it thousands of times.

    <Ctrl>+F then type U1 and BAM, U1 is now centered on your screen. No filters, no options, no modes, just a very simple, useful command.

     Tom

    • Post Points: 20
  • Wed, Jul 25 2012 6:32 AM

    • TH Designs
    • Top 25 Contributor
    • Joined on Fri, Apr 13 2012
    • Warminster, PA
    • Posts 269
    • Points 4,370
    Re: PCB Editor and "find" Reply
    ScottCad:

    To follow up

    It might be me, perhaps I am doing something wrong but I think there is a bug with this "Find" and display operation in 16.5

    I loaded up a design, clicked the Option pane then entered R1 in the entry box to find R1 on my board and the screen did not jump to the R1 location after hitting the enter key.

    In general edit Mode I right clicked "Super filter" and ticked Symbol/pin and then did a find and every time the screen auto pans to the location of the symbol. Even using the more option under find and selecting multiple symbols jumps the display to where they are.

    None of this worked before I set the superfilter to symbol/pin, in other words if the superfilter is turned off in GE mode then find is not working correctly.

    Would love to know if you guys are seeing the same thing at your end.

    I dunno if this is how the find is meant to work or not, but the sucker is not working right for me without invoking the superfilter as a first step..

    It's really wierd.. Dont make sense.

    Thanks Scott

    Scott,

    I have the same results. I didn't even know there was a "super filter". Silly me, I was just selecting the symbol and pins in what I suppose is just the regular "filter" box.

    I'm going to go through all of the responses and try each one and make a list of what works and what doesn't (on my computer)

    • Post Points: 5
  • Wed, Jul 25 2012 6:43 AM

    • TH Designs
    • Top 25 Contributor
    • Joined on Fri, Apr 13 2012
    • Warminster, PA
    • Posts 269
    • Points 4,370
    Re: PCB Editor and "find" Reply
    steve:

    Finding parts has three ways.

    1. Invoke a command in PCB Editor like Display Highlight or Display Assign Color then in the FInd by name type the refdes of the part you want and hit tab or return and the part is highlighted and zoomed to.

    2. No active command type the refdes in the Find by name, it is shown in the world view, then click on the Zoom to selection icon.

    For both of these to work you need to make sure that Symbols are checked in the Find Filter.

    3. No active command - left mouse button the part in the schematic and it zooms to object in the PCB.

    You can also type refdes <refdesname> hit return at the command line and the part is selected then use zoom to selection icon.

    You could also raise an enhancment request with Cadence / VAR to Improve this function..... 

    Hi Steve,

    My results from your suggestions:

    1. Display highlight then type refdes in find by name box: The first couple of times I tried this, it didn't work. Then I tried the suggestion from Scott on the "super filter" which worked. Came back and tried your method (superfilter is NOT set) and it now works every time. It works in all three modes, EE, PE, GE. This has been typical of my experiences with 16.5. One time something works, another time it doesn't. I'm sure it is me not being in the right mode or having some filter or option selected so I chalk those "mystery" operations up to my inexperience.

    2. Using world view window: I stumbled onto this one yesterday and it seems to work. (Is there anyway to clear the world view as it tends to get a bit cluttered)

    3. I have not been able to do this. I have ITC enabled, but the operation of ITC on my system has been sketchy at best.

    Thanks for the help,

     Tom

    • Post Points: 5
  • Wed, Jul 25 2012 6:43 AM

    • TH Designs
    • Top 25 Contributor
    • Joined on Fri, Apr 13 2012
    • Warminster, PA
    • Posts 269
    • Points 4,370
    Re: PCB Editor and "find" Reply
    steve:

    Finding parts has three ways.

    1. Invoke a command in PCB Editor like Display Highlight or Display Assign Color then in the FInd by name type the refdes of the part you want and hit tab or return and the part is highlighted and zoomed to.

    2. No active command type the refdes in the Find by name, it is shown in the world view, then click on the Zoom to selection icon.

    For both of these to work you need to make sure that Symbols are checked in the Find Filter.

    3. No active command - left mouse button the part in the schematic and it zooms to object in the PCB.

    You can also type refdes <refdesname> hit return at the command line and the part is selected then use zoom to selection icon.

    You could also raise an enhancment request with Cadence / VAR to Improve this function..... 

    Hi Steve,

    My results from your suggestions:

    1. Display highlight then type refdes in find by name box: The first couple of times I tried this, it didn't work. Then I tried the suggestion from Scott on the "super filter" which worked. Came back and tried your method (superfilter is NOT set) and it now works every time. It works in all three modes, EE, PE, GE. This has been typical of my experiences with 16.5. One time something works, another time it doesn't. I'm sure it is me not being in the right mode or having some filter or option selected so I chalk those "mystery" operations up to my inexperience.

    2. Using world view window: I stumbled onto this one yesterday and it seems to work. (Is there anyway to clear the world view as it tends to get a bit cluttered)

    3. I have not been able to do this. I have ITC enabled, but the operation of ITC on my system has been sketchy at best.

    Thanks for the help,

     Tom

    • Post Points: 20
  • Wed, Jul 25 2012 7:33 AM

    • mcatramb91
    • Top 75 Contributor
    • Joined on Thu, Jan 3 2013
    • Chelmsford, MA
    • Posts 95
    • Points 4,920
    Re: PCB Editor and "find" Reply

    I thought you were talking about Cadence Allegro 15.7 which never had the <ctrl>+F functionality, I didn't realize that you were talking about OrCAD Layout.  There are ways to do the same type of thing without having to go into the Super Filter or even the Find Filter to get it to happen.  It is certainly a good idea to submit an enhancement request to bring forward the <Ctrl>+F functionality for the old OrCAD Layout into Cadence Allegro.

    Mike

    • Post Points: 5
  • Wed, Jul 25 2012 8:04 AM

    • mcatramb91
    • Top 75 Contributor
    • Joined on Thu, Jan 3 2013
    • Chelmsford, MA
    • Posts 95
    • Points 4,920
    Re: PCB Editor and "find" Reply

    I have used this fillin confirmer box functionality in the past to gather information from the user.   I was able to easily generate an alias to allow you to use <Ctrl> + F to find components.  Each one of the commands below can be typed on the Allegro command line individually and I simply combined them into one alias mapped to <Ctrl> + F, here is what the alias looks like:

    alias ~F "prepopup ; pop dyn_option_select 'Selection set@:@Clear all selections' ; prompt 'Enter Ref Des' ; refdes $prompt ; zoom selection"

    The first command prepopup ; pop dyn_option_select 'Selection set@:@Clear all selections' clears all other selections so you center on one element instead of several.

    The second command prompt 'Enter Ref Des' opens a fillin confirmer box so you can enter the Ref Des you are trying to find.

    The third command refdes $prompt selects the Ref Des entered in the previous step in the design.

    The forth command zoom selection will zoom and center on the Ref Des

    You can add the Alias line above to your Allegro env file which is located in your PCBENV Folder so it will always be available during every Allegro session.  This may give you what you are looking for the short term and maybe Cadence can productize a solution in the tool out of the box.

    I attached a Text Document with the exact alias syntax in case the formatting get messed up after posting.

    Great Thread!

    Hope this helps,
    Mike Catrambone
    Plexus Engineering Solutions

    • Post Points: 50
  • Wed, Jul 25 2012 8:13 AM

    • ScottCad
    • Top 50 Contributor
    • Joined on Sat, May 26 2012
    • Roswell, GA
    • Posts 176
    • Points 2,775
    Re: PCB Editor and "find" Reply

    Tom to disable World View go to the toolbar and select View > Window, un-check what you dont need

    Thanks Scott

    • Post Points: 5
  • Wed, Jul 25 2012 8:46 AM

    • steve
    • Top 10 Contributor
    • Joined on Fri, Jul 18 2008
    • Woking, Surrey
    • Posts 1,162
    • Points 18,880
    Re: PCB Editor and "find" Reply

    Good job Mike this is very useful but.... (sorry there is always one of these), When I set this up in pcbenv and restart PCB Editor the CTRL + F doesn't work the first time I get E prompt Variable nor defined but If I do it again it works..... and secondly the clear all selections doesn't appear to work, I can find say C1 then CTRL + F again and C1 is still selected.... Maybe Cadence can add this to the new release (but fixed).......

    • Post Points: 20
  • Wed, Jul 25 2012 9:04 AM

    • Randy R
    • Top 50 Contributor
    • Joined on Wed, Jul 16 2008
    • Dupont, WA
    • Posts 192
    • Points 3,025
    Re: PCB Editor and "find" Reply

    Nice job Mike, but the Clear All Selections isn't working for me either.  I tried recording the script of clearing all selections and the syntax looks correct; but it's not working.

    Good Day, R².
    • Post Points: 20
Page 2 of 3 (37 items) < Previous 1 2 3 Next >
Sort Posts:
Started by TH Designs at 24 Jul 2012 09:00 AM. Topic has 36 replies.