10 Replies Latest reply on Jul 21, 2013 11:32 PM by david.hughes3

    Warning Labels




      We have a number of Warning Labels and Legal statements that we need to include on some of our schematics, these live in our central library.

      When they are placed on a schematic sheet they inherit electrical properties, as a resistor would, and therefore appear as follows:



      What property do we need to assign to this type of non-electrical symbol to stop DxDesigner seeing it as an electrical part?


        • 1. Re: Warning Labels

          Make them 'Annotate' type symbols, they look like they're of type 'Module' at the moment, which is used for physical components on the PCB.

          • 2. Re: Warning Labels

            Hi Rob,


            I have tried setting the symbol to be "Annotate" (see below) but the symbol still seems to be of an electrical type (allowing the Cluster and Exclude properties to be assigned)





            • 3. Re: Warning Labels

              I don't know of a way to keep symbol type properties from a symbol. Setting the symbol to ANNOTATE will keep the symbol from the netlist and partlist but it doesn't disallow adding symbol type properties.


              Properties are created with an "Attach to" attribute.  That attribute can be any combination of Symbol, Net & Pin.  There isn't a differentiation between Composite, Module or Annotate type symbols.


              How are the Cluster and Exclude properties beign assigned? How is this symbol being placed? Are you placing the part or the symbol? Using licensed DxDataBook?

              • 4. Re: Warning Labels

                Hi Mentor Shannonk - Thanks for your reply.


                We are placing the symbols from our central library and running an old Mentor (2009 ish) script to propagate the define properties from the hierarchical symbol down through to the components below. It seems that the script is putting the references onto every item below not just the components.


                Mentor Graphics have been in touch and have concluded the only way forward is to rewrite the script or abandon the plan



                • 5. Re: Warning Labels



                  Try this:


                  1. Create your hazard or logo graphic and save it as a BMP or JPG image file.

                  2. Open Symbol Editor, start a new symbol

                  3. File menu>Symbol>Add Picture....

                  4. Browse to the BMP or JPG created instep 1

                  5. Place image

                  6. Update symbol outline (may need to draw rectangle around image prior to this step) and move symbol origin point to lower left corner

                  7. Change properties as shown in the image (i.e. Annotate type of symbol, Forward to PCB=False; delete any other PCB Properties or Model properties)

                  8. Save the symbol.


                  Graphic Symbol Construction.JPG

                  • 6. Re: Warning Labels



                    Just make sure the graphic symbol is "Annotate", not Pin, Composite or Module.


                    Also make sure the Forward to PCB property is set to False.


                    Delete any other properties from the symbol. Right click on the property and you'll see an "X" on the right side; click it and the property is removed.


                    If your script adds the properties to the instantiated (i.e. placed in the schematic) symbol, delete these properties (or their values) at the schematic level.


                    Since your script is dealing with hierarchical properties, you may be able to limit the influence of the script by adding a LEVEL property to the hazard symbol. I'm not familiar with the use of the LEVEL property but I thought it might offer you a way of excluding this symbol from the generated outputs.





                    • 7. Re: Warning Labels

                      They have all of this working, the symbol is good, the graphics are good, the symbol type is good, the issue is a script that annotates a couple of properties on to each symbol as it is placed. So the solution would be to modify the script to recognize the different symbol types and only add the properties if the symbol type is module.


                      I don't know if this is possible, but the script is where the issue is.

                      • 8. Re: Warning Labels

                        Why worry about the script? Simply delete the properties it adds to the Annotate symbol.

                        • 9. Re: Warning Labels

                          Hi Mike,


                          Thanks for your time in trying to get this sorted for me. Mentor_Shannonk is correct in that our symbol is already drawn and added to our library and has the properties you mention added to it. The issue is with the script. We can still use the script and just delete the properties on the symbols we did not them added to, but my assumption was that the script would only append properties to electrical components and not just everything.


                          I have looked into the "LEVEL" property but do not think that this is going help - but worth a look anyway



                          • 10. Re: Warning Labels

                            I have finally worked out what to do to resolve the issue.....


                            The Mentor Script that propagates the properties seems to read the speccomp.ini file, so that things like power, grounds, on page & off page symbols do not get annotated. Therefore I have added all of our borders and statement symbols to this list and it seems to work a treat.


                            Many Thanks for all of your help with this