Pin layout doubt

Discussion in 'The Projects Forum' started by adriano08, Jun 25, 2010.

  1. adriano08

    Thread Starter Member

    Apr 25, 2010
    33
    1
    Hi. I have a doubt here for the eagle software.

    The pin layout for the IC in the library is different from what I read in the datasheet. I mean they designed in such a way that make your connection more easier I think.

    Example:
    Actual 555 pin layout:
    1- -8
    2- -7
    3- -6
    4- -5

    *Then in eagle one the pin layout of that is slightly different. For those using eagle software maybe you know what I mean. :)

    So I wonder if I do pcb fabrication, do I just do the normal way that is to solder all the components directly in if I were to do a small astable circuit? As the actual pin layout is different from software and in actual, I fret that something are wrong...

    Anyone can enlighten me?:confused:
     
  2. retched

    AAC Fanatic!

    Dec 5, 2009
    5,201
    312
    Is your pin layout backwards? If so, you may be looking from the bottom view.

    Also, is this in the schematic view or the PCB view?

    The schematic view, you can arrange the pins around to make the schematic easier to read, but on the PCB layout, it should be correct to match the IC.
     
  3. adriano08

    Thread Starter Member

    Apr 25, 2010
    33
    1
    Looking at the top view where there is the IC wording...

    In schematic view, the IC pin is different. What I did was just to add a component in and start wiring the nets.. Then after the all work in my schematic making, I switch it to board.

    I am not sure whether it will match because I had just fabricated one out. It look exactly the same design in what I routed in PCB.

    So is it that when in schematic view, the pin layout maybe different but when you are in the PCB view, it switch to standard pin layout? Or otherwise?
     
  4. Wendy

    Moderator

    Mar 24, 2008
    20,765
    2,535
    Schematics rarely show PCB layout (though there are exceptions). Schematics are meant to be easy to read. When I draw a schematic I put the pin numbers next to the black box I am drawing in the schematic (or op amp, or whatever). It is up to the user to interpret the drawing and make the transition to the PCB layout.

    Have you looked at the AAC ebook experiments? It shows both, the layout and the schematic in an easy to read format. You can access them looking at the top of this page.
     
  5. mcgyvr

    AAC Fanatic!

    Oct 15, 2009
    4,769
    969
    most (if not all) PCB/Schematic capture programs do associate the schematic pins with the layout pins (or attached pattern) though obviously. So if your schematic pins are incorrect your layout will be too. Get it right from the start to avoid confusion down the road. I don't us Eagle (thank god) so I am probably missing something.
     
  6. jpanhalt

    AAC Fanatic!

    Jan 18, 2008
    5,675
    899
    No, that is not quite how it works in Eagle. Several IC's have the location of the pins on the schematic symbol different from the board symbol/package. That happens with all of the logic chips (use invoke to see the supply pins, but they are not on the chip symbol at all). The 555 is another case. If you look around, I recall there is a version with the pins on the schematic symbol in the same order as on the chip. The pin numbers, labels, and functions are correct. And the pins are linked to the proper pins on the device package.

    One thing that you do have to watch out for is an inversion that occurs when you move from component side to the copper side on the PCB, but that should not be unique to Eagle and is probably beyond the scope of the OP's question.

    John
     
  7. mcgyvr

    AAC Fanatic!

    Oct 15, 2009
    4,769
    969
    I misunderstood the post.. I was thinking his schmatic pins (for example if IC Vcc is pin 8) that the schematic had it to pin 2 or whatver.
    It really doesn't matter how the schematic is drawn or how the pins are organized within the schematic symbol as long as the correct pin on the schematic is pointing to the correct pin on the pad layout. The pad layout must be correct but the schematic symbol can put those pins anywhere you want as long as 1=1, 2=2,etc...
     
  8. n1ist

    Active Member

    Mar 8, 2009
    171
    16
    When creating schematic symbols, there are certain conventions:
    - Power on the top
    - Inputs on the left
    - Outputs on the right
    - Ground and negative supplies on the bottom
    - Pins grouped in some sort of logical or functional blocks
    These help make the schematic readable.

    When creating PCB footprints, you have to follow the layout of the real part.
    /mike
     
  9. jpanhalt

    AAC Fanatic!

    Jan 18, 2008
    5,675
    899
    Nice plan, but here is one version of the 555 that may have sparked this question and doesn't quite fit it:

    [​IMG]

    Why it is drawn like that, I have no idea.

    John
     
  10. SgtWookie

    Expert

    Jul 17, 2007
    22,182
    1,728
    I usually use the ICM7555 in one of the Maxim libraries. It's schematic pins are grouped more logically (making your schematics neater), however on the PCB side, the signals go to the correct pins.

    If you use the Mirror tool on an IC in the board layout editor, you'll see the NAME and VALUE fields reversed. This is because it's been sent from the top layer to the bottom layer, or vice versa. If you mirror a critter that has more than 3 legs, odds are very good that you'll have to insert it from the opposite side of the board than it was before you mirrored it.

    This is a handy way to send SMD/SMT items to the bottom of the board, if you only want to make a single-sided board and have mixed SMD/SMT with thru-hole parts.
     
  11. jpanhalt

    AAC Fanatic!

    Jan 18, 2008
    5,675
    899
    That also applies to 3-pin devices when the pins are not in a line, unless the pins are long enough to be bent. That is practical for many leaded devices (e.g., TO-93), but not for packages like the TO-3 package. Of course, for the microscopic SMD 3-pins devices it does flip the board side as suggested, but be careful. The program may already have assumed you would be mounting an SMD on the copper side, and a mirror will put the device on the wrong side for SMD's. Eagle will follow that potential problem and do such things as insert vias or give you a layer violation.

    The ST NE555 also has a logical layout.

    John
     
  12. SgtWookie

    Expert

    Jul 17, 2007
    22,182
    1,728
    John,
    I'm sure you meant TO-92 devices instead of TO-93.
    Even if pins ARE in line, if you mirror such devices as a TO-220 MOSFET, you better insert it from the correct side of the board (if the text is mirrored, it needs to be inserted from the bottom).

    Sometimes it just makes a lot of sense to send parts to the other side of the board, such as when you'd have to run a lot of jumpers.

    The default libraries have all of the SMD/SMT devices on the top layer. It would be a good practice to continue that basic premise when developing new library models. It only takes two clicks to send a part to the other side of the board (mirror tool, click on part).
     
  13. jpanhalt

    AAC Fanatic!

    Jan 18, 2008
    5,675
    899
    Yep, I meant TO-92.

    The point I was trying to make, if pins are in a line, regardless of number, is that because there is an axis of symmetry going right though the pins (consider the TO-220) a mirror image will not affect the side of the board from which the device must be inserted to satisfy the electronic constraints. However, possible spacing issues due to asymmetry of the body and/or heatsink relative to the pins may occur.

    When I play mirror games with such devices, I usually make a new device with an x or dot at pin 1. That helps me keep track of what is going on and the space I may need for the heatsink, etc. My earlier comment about being outside the scope of the OP's question was directed at these mirror issues.

    John
     
Loading...