+ Post New Thread
Page 1 of 2 1 2 LastLast
Results 1 to 20 of 22
  1. #1
    Newbie level 5
    Points: 456, Level: 4

    Join Date
    Oct 2010
    Posts
    10
    Helped
    3 / 3
    Points
    456
    Level
    4

    Why pad size smaller than hole size when in gerber file

    Hi

    is anyone there know why the pad size become smaller than the hole size when in gerber file? I used dxp protel 2006 to design pcb. In layout, my pad size is bigger than the hole size, but when in gerber file, the opposite situation occurred. Is there anyone can help me solve this kind of problem?

    Helpless

    •   AltAdvertisement

        
       

  2. #2
    Advanced Member level 2
    Points: 5,545, Level: 17
    Achievements:
    7 years registered

    Join Date
    Dec 2006
    Location
    India
    Posts
    515
    Helped
    89 / 89
    Points
    5,545
    Level
    17

    Re: Why pad size smaller than hole size when in gerber file

    Which CAM tool you are using to view gerbers.
    this might be because you ddont have set the NC drill table properly you have to set the drill sizes in CAM tool similar to that used in PCB.


    1 members found this post helpful.

  3. #3
    Advanced Member level 3
    Points: 9,635, Level: 23
    cyberrat's Avatar
    Join Date
    Jun 2001
    Location
    In the sewers of the U.K.
    Posts
    889
    Helped
    85 / 85
    Points
    9,635
    Level
    23

    Re: Why pad size smaller than hole size when in gerber file

    Or because you have not used RS274-X and have not entered your aperture sizes correctly?
    Please do not PM me questions that are better asked in the PCB forum :)


    1 members found this post helpful.

  4. #4
    Super Moderator
    Points: 50,045, Level: 54
    Achievements:
    7 years registered
    keith1200rs's Avatar
    Join Date
    Oct 2009
    Location
    Yorkshire, UK
    Posts
    10,877
    Helped
    2075 / 2075
    Points
    50,045
    Level
    54

    Re: Why pad size smaller than hole size when in gerber file

    Just to add something here, Amy has sent me the Gerber & drill files which I have loaded with GCprevue and the holes are definitely the wrong size (a fact confirmed by the PCB fabricator). Unfortunately it is not a simple matter on number of digits or units. I don't know Protel so have run out of ideas although we have tried several times to correct this. I am fairly sure it is too with how the drill files are created.

    We need a Protel expert!

    Keith


    2 members found this post helpful.

  5. #5
    Super Moderator
    Points: 260,224, Level: 100
    Awards:
    1st Helpful Member

    Join Date
    Jan 2008
    Location
    Bochum, Germany
    Posts
    45,442
    Helped
    13826 / 13826
    Points
    260,224
    Level
    100

    Re: Why pad size smaller than hole size when in gerber file

    You should give some more information. Which file formats are you using for NC (provided, that the drill size is the problem, as Keith reported)? Does the file format include tool sizes with the drill data?

    If I remember right, the default Protel/Altium workflow doesn't lead you to include the tool data during drill file generation. Because I'm only occasionally working with Altium, I simply added the sizes in a gerber tool, instead of further investigating the issue.


    1 members found this post helpful.

  6. #6
    Newbie level 5
    Points: 456, Level: 4

    Join Date
    Oct 2010
    Posts
    10
    Helped
    3 / 3
    Points
    456
    Level
    4

    Re: Why pad size smaller than hole size when in gerber file

    I used RS-274-X format. no, the tool sizes is separated from the drill data. but result still wrong. Is there have any setting during save the drill drawing. Coz yesterday Keith give me the manual for gerber file cretaed. But it din mention about the drill drawing. And is the setting for gerber file have something wrong. Please help me ..


    1 members found this post helpful.

  7. #7
    Full Member level 4
    Points: 3,038, Level: 12
    Achievements:
    7 years registered

    Join Date
    Jun 2010
    Location
    INDIA
    Posts
    199
    Helped
    78 / 78
    Points
    3,038
    Level
    12

    Re: Why pad size smaller than hole size when in gerber file

    is this issue available for all thru hole pads?? or to some particular pads??
    for the first case we can suspect ncdrill generation methods or gcprevue.
    if proble is occuring with some particular pads means some issue is there with your library/padstack.
    Open the geber in GCprevue and check the property of copper pad in top layer,ensure it is same as the PCB data.
    You can open the ncdrill file ( hole info) using a notepad and can ensure whether the data is correct.
    If possible can you share the gerber files along with ncdrill data?


    2 members found this post helpful.

  8. #8
    Newbie level 5
    Points: 456, Level: 4

    Join Date
    Oct 2010
    Posts
    10
    Helped
    3 / 3
    Points
    456
    Level
    4

    Re: Why pad size smaller than hole size when in gerber file

    Hi, i still cannot install the GCprevue yet. So, still cannot check the drill file by myself. I can share the file, but the problem is i dono how to share it here?
    Please Help me..


    1 members found this post helpful.

  9. #9
    Full Member level 4
    Points: 3,038, Level: 12
    Achievements:
    7 years registered

    Join Date
    Jun 2010
    Location
    INDIA
    Posts
    199
    Helped
    78 / 78
    Points
    3,038
    Level
    12

    Re: Why pad size smaller than hole size when in gerber file

    Quote Originally Posted by amy87 View Post
    Hi, i still cannot install the GCprevue yet. So, still cannot check the drill file by myself. I can share the file, but the problem is i dono how to share it here?
    Please Help me..
    you can use any gerber viewer to check the gerber. GCprevue is a free ware.
    gcprevue down load link: GraphiCode - The Original Gerber viewer

    to share the files you first zip all gerber files ( top,bot,silk,...) using winzip or win rar . then click on the Go advanced button . there you will get options to upload files.


    2 members found this post helpful.

  10. #10
    Newbie level 5
    Points: 456, Level: 4

    Join Date
    Oct 2010
    Posts
    10
    Helped
    3 / 3
    Points
    456
    Level
    4

    Re: Why pad size smaller than hole size when in gerber file

    Ok, i post the drill file and gerber file here. Hope can help me ...


    1 members found this post helpful.

    •   AltAdvertisement

        
       

  11. #11
    Full Member level 4
    Points: 3,038, Level: 12
    Achievements:
    7 years registered

    Join Date
    Jun 2010
    Location
    INDIA
    Posts
    199
    Helped
    78 / 78
    Points
    3,038
    Level
    12

    Re: Why pad size smaller than hole size when in gerber file

    hi Amy,

    issue is with your CAD data itself.
    check the file "C:\Users\Amy\Documents\NEW\cam1.rpt" or 'cam1.drl' . it says you have 28 different types of drills I think some mistake is there in your ncdrill generation (.drl file) procedure.
    as per this data the smallest drill size in your design is 0.050"(1.27 mm) and it is for vias!!!
    Please check the .drl generation procedure again..



  12. #12
    Super Moderator
    Points: 50,045, Level: 54
    Achievements:
    7 years registered
    keith1200rs's Avatar
    Join Date
    Oct 2009
    Location
    Yorkshire, UK
    Posts
    10,877
    Helped
    2075 / 2075
    Points
    50,045
    Level
    54

    Re: Why pad size smaller than hole size when in gerber file

    Yes, I double checked the drill files to make sure GCprevue was showing me the correct values (it sometimes lies) and found the same thing. Unfortunately I don't know Protel so cannot talk Amy through fixing it.

    Keith



  13. #13
    Super Moderator
    Points: 260,224, Level: 100
    Awards:
    1st Helpful Member

    Join Date
    Jan 2008
    Location
    Bochum, Germany
    Posts
    45,442
    Helped
    13826 / 13826
    Points
    260,224
    Level
    100

    Re: Why pad size smaller than hole size when in gerber file

    I agree, that the fault is apparently already present in the Protel design. I scaled cam1.drl to 50% and got partly reasonable drill sizes. There are however several details that aren't manufacturable as is, e.g. multiple drills in a pad. I also don't understand, why there are 14 different drill files have been produced, most of them empty. The four containing data are almost identical, except for an obviously erratic drill in a SMD pad.

    The PCB outline is apparently missing from the gerber plots, it would be expected in *.gm15 according to Protel/Altium standard.

    I must add, that I'm no used to operating Protel with imperial (inch) units, the drill size confusion may be related to it.

    To make us understand the nature of the problem, you should possible show a screenshot of the layout, or post 68_design.pcbdoc.



    P.S.: To add a more general comment: I seriously doubt, if the design will work reliably with the present supply and ground wiring and effectively no bypass caps near to most logic and memory ICs. It's also strongly recommended to use wider traces for power supply. When making logic circuits on a two-layer PCB, I would always try to wire a least ground and possibly vcc in a grid topology.
    Last edited by FvM; 30th October 2010 at 10:13.



  14. #14
    Newbie level 5
    Points: 456, Level: 4

    Join Date
    Oct 2010
    Posts
    10
    Helped
    3 / 3
    Points
    456
    Level
    4

    Re: Why pad size smaller than hole size when in gerber file

    Act I dono where can change dy. There are not many step need to do in order to create the gerber file. But about the drill file, i din set any thing because dono where can do setting. Can tell me where can do the setting?



  15. #15
    Full Member level 4
    Points: 3,038, Level: 12
    Achievements:
    7 years registered

    Join Date
    Jun 2010
    Location
    INDIA
    Posts
    199
    Helped
    78 / 78
    Points
    3,038
    Level
    12

    Re: Why pad size smaller than hole size when in gerber file

    check the link
    https://www.edaboard.com/thread12042.html
    hope this will work for you.

    If everything fails means simply edit the values in cam1.drl using a text editor and save it (eg:T28C0.0500 means Tcode 28 with 0.050" drill dia edit it to T28C0.0100 ie Tcode 28 with 0.010" drill dia)



  16. #16
    Advanced Member level 3
    Points: 9,635, Level: 23
    cyberrat's Avatar
    Join Date
    Jun 2001
    Location
    In the sewers of the U.K.
    Posts
    889
    Helped
    85 / 85
    Points
    9,635
    Level
    23

    Re: Why pad size smaller than hole size when in gerber file

    Have you done a drill drawing to let the manufacturer know what size holes on what pads you want?

    Edit: Why so many drill files?

    Surely you only need 2, 1 for plated and one for non plated.
    Last edited by cyberrat; 30th October 2010 at 11:50.
    Please do not PM me questions that are better asked in the PCB forum :)



  17. #17
    Newbie level 5
    Points: 456, Level: 4

    Join Date
    Oct 2010
    Posts
    10
    Helped
    3 / 3
    Points
    456
    Level
    4

    Re: Why pad size smaller than hole size when in gerber file

    pcb file.zipThanks for help. I post the pcb file here... Hope can find the actual problem through it. Cause act the setting followed the instruction dy. The problem still occurred at all.



  18. #18
    Super Moderator
    Points: 260,224, Level: 100
    Awards:
    1st Helpful Member

    Join Date
    Jan 2008
    Location
    Bochum, Germany
    Posts
    45,442
    Helped
    13826 / 13826
    Points
    260,224
    Level
    100

    Re: Why pad size smaller than hole size when in gerber file

    Unfortunately, I don't have the said Protel version. With recent Altium versions, the drill tools are apparently assigned correctly. So I wonder, if it's a problem of a specific Protel version.



    There seems to be a change in the processing of the milled J1 slots, Altium sees only two drills at the slot ends. The three drills for each pad in your drill file version cause possibly problems in PCB manufacturing, as already mentioned. Personally, I prefer larger round pads for those DC connectors, because they can be produced by any manufacturer without problems.
    Last edited by FvM; 31st October 2010 at 00:12.



    •   AltAdvertisement

        
       

  19. #19
    Newbie level 5
    Points: 456, Level: 4

    Join Date
    Oct 2010
    Posts
    10
    Helped
    3 / 3
    Points
    456
    Level
    4

    Re: Why pad size smaller than hole size when in gerber file

    Hi,

    I think before this i misunderstand already. I direct save the drill file from gerber file (camtastic) there, so the size of drill act is the total size for hole and pad. Now, i save the drill file from NC drill file there, the size is correct. So, izzit means that wehave one drill file only?



  20. #20
    Super Moderator
    Points: 260,224, Level: 100
    Awards:
    1st Helpful Member

    Join Date
    Jan 2008
    Location
    Bochum, Germany
    Posts
    45,442
    Helped
    13826 / 13826
    Points
    260,224
    Level
    100

    Re: Why pad size smaller than hole size when in gerber file

    As far as I see, you don't have unplated holes in your design, so one NC drill file is correct.

    But you should define a board outline in your Protel design, and check, if the PCB manufacturer
    can make milled throughplated slots for connector J1 from your present drill data.



--[[ ]]--