Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Silk Screen Text not appearing (OrCAD 16.3)

Status
Not open for further replies.

hobbss

Member level 2
Joined
Oct 18, 2010
Messages
49
Helped
20
Reputation
40
Reaction score
19
Trophy points
1,288
Activity points
1,858
I am attempting to create a silk screen for my pcb in OrCAD 16.3.

I have tried two methods:

1. Manually selecting all of the silk screen subclasses with the display color editor, and then adding a new layer to the artwork tab

2. Running the silk screen generator (sorry for using an Expedition term), which, as I understand it, grabs all the silkscreen subclasses and dumps them in a single class "autosilk_top".

In both cases, I can see both the component outlines, pin 1 designators, manual text, and refdes's on the screen (i.e., when only "autosilk_top" is enabled). However, when I create the artwork, the text never makes it through. All of the component outlines, the pin 1 designators, et al make it to the art file. However, absolutely no text (either refdes's or my manual text) makes it through. Is this because my text doesn't have "width"? If so, how do I add width?

Is there something else I am missing?

---------- Post added at 09:31 ---------- Previous post was at 08:58 ----------

Follow up:

To anyone who has this problem:

I am unsure if this is the "right" way to do it, but it seems to work.

The text has zero width by default. It seems like this is most likely an error I made when I created the footprints (for the refdes's), and the manual text (i.e., rev number), when I added it to the board.

I ran the auto silk generator. I then turned off all objects but the autosilk_top layer. I set my find filter to text only. I selected all of the text on the board, and went to Quick Utilities --> Design Parameters. On the text tab, I selected Setup Text Sizes. In the resultant window, I set the Photo Width field to 5 for all of the text. The next time I created the silk screen layer art file, it had all of my text.

For the record, it would be nice if the log file denoted that it was throwing a way text due to zero width (like it does for lines)...
 

mashak

Junior Member level 3
Joined
Dec 12, 2007
Messages
28
Helped
6
Reputation
12
Reaction score
6
Trophy points
1,283
Activity points
1,437
Changing the text parameters in PCB Editor is one way of getting that. But There was nothing wrong when you created the library with 0 width text.

Most of us do the same way.

The only thing what you have to do while generating the gerbers is that. Select the silk film and there are few options shown on the right side , in that there is something called as "Undefined line width" You have to set that to 6 mill or the value you fill OK with. Them when you generate the Artwork you will have all the 0 width converted to the value specified by you.

By following this method you will have all the text with a uniform width.

---------- Post added at 07:51 ---------- Previous post was at 07:50 ----------

Changing the text parameters in PCB Editor is one way of getting that. But There was nothing wrong when you created the library with 0 width text.

Most of us Create the library the same way.

The only thing what you have to do while generating the gerbers is that. Select the silk film and there are few options shown on the right side , in that there is something called as "Undefined line width" You have to set that to 6 mill or the value you fill OK with. Them when you generate the Artwork you will have all the 0 width converted to the value specified by you.

By following this method you will have all the text with a uniform width.
 
  • Like
Reactions: hobbss

    hobbss

    Points: 2
    Helpful Answer Positive Rating

hobbss

Member level 2
Joined
Oct 18, 2010
Messages
49
Helped
20
Reputation
40
Reaction score
19
Trophy points
1,288
Activity points
1,858
Thanks for the tip. I like that method better than having to remember to edit all of the text in every design (and even more than going back to my library and changing all of the refdes's there). It also makes the design cleaner, because I can leave the refdes's as 0 width on the screen.
 

gopintj

Member level 4
Joined
Sep 1, 2010
Messages
77
Helped
4
Reputation
8
Reaction score
4
Trophy points
1,298
Location
Thirukalukalukundra, Kanchipuram, Tamilnadu, India
Activity points
1,953
Hi, I use CADENCE ALLEGRO 15.3

Hi, I too have the same problem. But, for me, even after changing the value of UNDEFINED LINE WIDTH to 6mm, i cant see the silk screen part in my art file. I first, tried to generate art file to show only my ETCH-TOP and ETCH-BOTTOM layer, then i tried PIN. After creating art file of these three, i could see the corresponding diagrams in VIEWMATE. But, i couldnt see the silk screen while i include it in ARTWORK->TOP list.
Should i have to add some more sub classes to see these silk screen..?
Could anyone please tell me what are the sub classes needed to be added to see the silk screen in my ART WORK?
And, What are the artwork layers i have to generate to convey them to fab house so that i can have my pcb back?
 

Status
Not open for further replies.

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top