OrCAD Layout Users-Generating Correct Gerber and Drill Files

Archive BatchPCB
1

Hello,

I’ve been rummaging through the forums for a few days now trying to gather information about generating correct OrCAD Layout Plus gerber files to use with SparkFun’s BatchPCB service. I’ve come a long way; however, there are still some issues that probably still need to be resolved. I couldn’t find any information on some issues I’ve been dealing with, so hopefully, this will help others with their experiences and help sparky’s life too.

According to the BatchPCB FAQ found here:

http://www.batchpcb.com/faq.php

The following Gerber files should be generating with Layout’s “Post Processor”:

Layer Name (OrCAD Gerber File Extension)

  • Top Copper Layer (*.TOP*)

    Top Solder Mask (.SMT)

    Top Silkscreen (.SST)

    Bottom Copper Layer (.BOT)

    Bottom Solder Mask (.SMB)

    Bottom Silkscreen (.SSB)

    Drill File (thruhole.tap and/or thruhole.npt) – More On this Later


    • I found a post by ‘mike’ found [here that also includes the Assembly Top (.AST), and Drill Type Summary Report (.DTS).

    Question 1:

    The only reason (I can find) for including the Assembly Top (.AST) layer, is the board outline (usually defined on Layer 0 Global). The board outline is merged into this layer and might help sparky panelize the board. However, from what I see, this isn’t really needed if we duplicate the obstacle board outline (as a detail obstacle type) on the Top Silkscreen (.SST) and Bottom Silkscreen (.SSB) layers. Using Top/Bottom Silkscreens to outline the board and for the purpose of streamlining the whole process, would it be safe to omit the Assembly Top (.AST) layer?

    Question 2:

    I’ve taken a look at the Drill Type Summary Report (.DTS) file and this is what it looks like:

    ******************************
*                            *
* DRILL TAPE SUMMARY REPORT  *
*                            *
* C:\PATH_TO_MAXFILE.MAX     *
* Tue Apr 25 05:18:53 2006   *
*                            *
******************************

TOOL     SIZE     QUANTITY FEED     SPEED    
---------------------------------------------
T1       135      177      200      100      
T2       280      14       200      100      
T3       310      20       200      100      
T4       340      156      200      100      
T5       370      10       200      100      
T6       380      6        200      100      
T7       420      42       200      100      
T8       540      6        200      100      
T9       760      2        200      100      
T10      900      3        200      100      
T11      1250     4        200      100      
T12      1470     2        200      100

    After browsing the forums, I don’t see anything that looks like it should be included with the .zip submission and it isn’t mentioned on the FAQ. Do we really need this file to be included with our zip file submission? Also, after taking a closer look at my drills, it looks like my VIAs drills (T1) are 13.5 mils. These VIA drills be increased to 20 mills minimum (for BatchPCB) correct?

    Question 3:

    It appears that the real drill information from OrCAD’s post processor can be found in two files: thruhole.tap and thruhole.npt and both appear to have the same drill coordinate/tool format. I’ve only found references to the thruhole.tap file in these forums, and this is definatly a file that needs to be included. However, I couldn’t find any references regarding the thruhole.npt file. After viewing this drill file in viewmate, it appears that the thruhole.npt file are non-plated thruhole drills. So my 3rd question is, since it would be desirable to have non-plated thruhole drills, how do we include this information in our submission to sparky?

    Thanks to those users who came before me. Thanks sparky for offering a low cost PCB service, and thanks in advance to those who respond.

    -Brian](http://www.sparkfun.com/cgi-bin/phpbb/viewtopic.php?t=1353&highlight=orcad)

    2

    i don’t think you need the DTS since all the drill bits and xy coordinates are defined in your drill files.

    also, you can merge the .top and .npt files if you go to the settings where you can turn on and off the layers you want to post process.

    (it is a check box that says merge drill files) and now you have one drill file that defines regular plated and nonplated thruholes.

    (i only used orcad once, so i maybe incorrect)

    3

    Hi Frdchang,

    Thanks for the reply. That’s useful tip. I merged the the top layer with the drill file. I still get the thruhole.tap file, and the thruhole.ntp file is now gone. :slight_smile:

    I’ve run my board through the DRC bot, and placed thruhole.tap as the drill file and it looks like everything went through fine.

    —As a side node and a useful tip for others—

    I do have one problem that I found with my board. The DRC bot fails with “Apature too thin” for a size of 0.002. I looked at this in the apature listing, and found a whole bunch of draws and coordinates for D29 0.002 apapture. I wasn’t going to go though each one and examine it, so I loaded the top layer into Viewmate, then changed changed the apature size, in my case Apapture D29 from 0.002 to 0.250 and it showed quite well where the apapture was being used on the board. Since I rotated a component at an odd angle (and it contained a square pad), Orcad used a 0.002 apapture to draw the square pad at an angle. They look a bit funky, heres a pic:

    http://cowboy.directgames.net:81/temp/orcad1.jpg

    Changing the apature size in the “Apapature” spreadsheet doesnt work and I don’t want to manually edit the gerber files. So I’m going to try and change the pad footprints/padstack to round and hopefully the problem will be solved.

    If anyone knows of a better way to fix a small apature problem in Orcad, let me know :wink:

    –Brian

    4

    Brian

    would it be safe to omit the Assembly Top (.AST) layer?

    I never send the AST layer or a DTS file.

    duplicate the obstacle board outline (as a detail obstacle type) on the Top Silkscreen (.SST) and Bottom Silkscreen (.SSB) layers

    You could do it that way…but to show a board outline in Orcad they have you turn it on for each layer. Go into Options/Post Processing settings…then tile them. You should see the pcb on the right side of the screen and the layers on the other. Click on the TOP layer and right click…from the options pick PREVIEW…you should see the pcb without a board outline. Now click on the COLOR SETTINGS button on the tool bar and you’ll see BOARD OUTLINE…pick a color and you should see the outline. Some companies I worked for just required the TOP and BOTTOM layers to have a outline…the company I do work for now requires all layers to have an outline shown.

    5

    Hi all I apologize for the ignorance. How exactly do you merge the drill files? I looked in the post process settings but could not find it.

    Thanks in advance,

    –Brian

    6

    Hello again,

    Zorakid:

    In OrCAD Layout, what I did was:

    Options > Post Process Settings… > Select *.TOP row, right click and click Properties…

    Then check “Combine Plated/Non-Plated Thru Holes”

    I’m not sure if what I did was totally correct (so someone can correct me if I’m wrong). Come to think of it, I probably should do it for all layers I’m submitting. Can anyone verify this?

    Cloudy:

    Thanks for the help! I’ve started to use the online DRC on BatchPCB, and have so far, my zip contains only .TOP, .BOT, .SST, .SSB, .SMT, .SMB, and drillfile thruhole.tap.

    However, the DRC bot is now mis-calculating the size of my 4x5 PCB and generating a price of $25,000 dollars. I’ll try the board outline trick to see if that solves the problem with the DRC! Thanks a bunch!

    7

    When I’m trying to upload my design on some website, they are asking me fore *.tap file but I actually have my drill file in *.drl format. Suggestions are appreciated.