Duplicate the RefDes 

You can add a duplicate RefDes to the Silkscreen and Assembly using Add > Text.

1) Add > Text
2) Change the Class to REFDES and Subclass to SILKSCREEN_TOP under the Options Tab
3) Select the component
4) Indicate text location and enter the current RefDes Text.

This text will be associated to the component and move with the component.  One word of caution, if you enter a different RefDes than what is current assigned to the component it will rename the RefDes to what you last entered.

I would always change the extra RefDes text to the DISPLAY_TOP subclass so I wouldn't have a duplicate RefDes on the SILKSCREEN_TOP subclass.  Just make sure to include the DISPLAY_TOP subclass with your silkscreen artwork film record.

I guess another alternative would be to update your library symbols with a RefDes place holder on the DISPLAY_TOP subclass and refresh the symbols using Place > Update Symbols.

Hope this helps,
Mike Catrambone
Plexus Engineering Solutions

Mike,  tried this and worked great.  Our boards generally have plenty of room, so I will usally over do the silkscreen layer with markings for whomever stuffs the board, duplicate RefDes on the silk screen is what I was looking for.  We share symbol libs, but not everyone shares my opinion of "more is better" in regards to silk, I'm hesitant to modify the symbols.   

MSC   9/7/12 

Hey Ron,

I do have a solution to generate special text for documentation and silkscreen associated to component. (I used the COMMENT property in the attached image)

1. Attach a property to component using Edit > Property.
2. Generate text on Class Manufacturing / Subclass Properties using Display > Property.
   • Select Graphics Tab and click on available property on the left to move it to the right
   • Adjust the Text Block and Manufacturing Subclass, can be any subclass, then click Create.
3. Use Edit > Change to move the newly added text to the Class / Subclass you wish and it will remain associated to the component when moving component.

Only downside is if the property is updated than you have to run thru the process above again because the text is not updated (Not Dynamic) 

Hope this helps,
Mike Catrambone
Plexus Engineering Solutions

The easy way I have found to do this is to use the Auto-Silk Function that is under the menu Manufacture > Silkscreen. Open that menu and choose Reference Designator to be silk. Set the other classes and subclasses to none. Click the silkscreen button and a duplicate reference dez will get placed on the Manufacturing Subclass of autosilk_top.

You might want to turn on that class in the color dialog so you can see the completed results and make the color something like green so it stands out, additionaly you may need to turn off your refdez under the component class as the auto silk can put the refdez in the exact same spot as it is on your silkscreen - component class layer.

With the duplicate of the reference dez on the autosilk_top layer you can change it's size or move it to a different subclass if you wish. You can also delete the duplicates you dont need. When you generate your gerbers dont forget to include the autosilk_top in your output for your silkscreen.

Hope this helps

Thanks Scott.

Ron my idea is a universal one. Now I verified what you mentioned about moving a part and I see what you mean about the text block snapping back to it's original size. To change this default try the following.

In the auto silkscreen dialog box check the following "Lock auto silk text for incremental updates" Believe that should get you where you need to be.

Thanks Scott.

Sorry for the slow response.  I used my method across the board in 100s of locations so I wouldn't consider it a solution for individual cases only.  To get the properties values loaded quickly I generate an incremental 3rd Party Netlist to add the properties to all the components all at once.  I created a user defined property (Setup > Property Definitions...) so it doesn't get mixed up with other properties that may already have values assigned.

Here is what the 3rd Party Netlist would look like:

$PACKAGES
$A_PROPERTIES
TOP_SILK   "DC_IN"     ;  TP31
BOT_SILK  "DC_OUT"  ;  TP900
$END

Use File > Import > Logic then select the Other tab to load the netlist above. (make sure that Supersede all logical data" is unchecked)

You could also add this property to the schematic and pass it forward to the layout. (remember you would need to setup the tool to pass the user defined property forward)

As far as moving a part which had the property value text changed reverting back to the original text, I don't see the text change in my method.  The only issue that I have is the text is not dynamic so if you change the property value it will not automatically update the text on the board so you have to go thru the property display process again or just rename the text.

Hope this helps,
Mike Catrambone
Plexus Engineering Solutions