EAGLE CAD LIB EDITOR TUTORIAL PART 3

[exxos]

This guide will (try to) explain how to create a simple part for a library. In this example I will create a PLCC44 ROM..


I know for a fact there is a PLCC44 "package" in one of the reference libs. So will we copy/paste that to save creating it from the ground up. I will explain how to do a new package in another guide another time...

So we load Eagle and load up the lib editor.

FILE - OPEN - LIBRARY

1.JPG (42.34 KiB) Viewed 4087 times

I use the "ref-packages.lbr" in this case. It's a very large lib of packages ready to rip.

2.JPG (119.52 KiB) Viewed 4087 times

Click the EDIT icon from the massive tool bar of nothingness...

7.JPG (48.69 KiB) Viewed 4087 times

Scroll down and look for the package we want. Which is the PLCC-44S. Basically PLCC package, 44 pins, Socketed type... Click OK..

3.JPG (38.96 KiB) Viewed 4087 times

Then your shown the socket package like below. This saves us a lot of work in not having to create all this ourselves! yay!

4.JPG (143.35 KiB) Viewed 4087 times

Using the GROUP tool, select the whole package as shown below.

(the group tool is the normal "rubber band" box type thingy like in windows etc)

5.JPG (128.11 KiB) Viewed 4087 times

Go into the EDIT menu and click COPY.

6.JPG (154.42 KiB) Viewed 4087 times

Now go into the FILE menu and click NEW..

Now we need to click the EDIT button and make sure it says PACKAGE at the top. If it doesn't, click the PAC button at the bottom.

In the text box ( near the bottom "new") I used PLCC44 as my package name. Type it in as shown below then click OK.

9.JPG (92.49 KiB) Viewed 4087 times

Another pointless box to click YES..

10.JPG (14.14 KiB) Viewed 4087 times

Now we need to click the GRID icon and put the options I did below. Of course if you are doing other parts, such as tiny SMT stuff, then a smaller grid such as 0.1mm is probably better.. But in this case. 1.27mm is a normal size to use.

11.JPG (105.46 KiB) Viewed 4087 times

Now go into the EDIT menu and click PASTE. It should now paste the part you copied earlier. Try to center it in the center of the grid so the "+" is in the middle of the part.

TIP: For some reason it lost my copied part, and it said the past buffer was empty If this happens, load up Eagle a second time and load the reference lib and do the copy again..

12.JPG (117.06 KiB) Viewed 4087 times

Now a WARNING here... Never EVER assume the reference packages are correct in any way shape or form. Print it out and confirm it. Look for datasheets and confirm its all right. Never EVER assume the pads are all aligned properly, CHECK EVERYTHING!

Use the INFO tool and click pin1 on the PLCC package. Confirm it says 1 in the NAME part in the pop up box. CHECK THEM ALL! Leave nothing to chance. Confirm all the pin numbers are correct!

If any pin numbers are wrong, simply change them in the NAME box.

13.JPG (118.62 KiB) Viewed 4087 times

[exxos]

Now lets do some small tweaks so we can at least say we wasn't 100% lazy with the editor..

Click the INFO TOOL and click the top border line of the package... We do this just to see what layer it is on , in this case layer 21 Tplace. Click cancel.

d1.JPG (130.36 KiB) Viewed 4086 times

Now click the CIRCLE TOOL..

Make sure Layer 21 is selected in the layer select menu also.

d2.JPG (135.22 KiB) Viewed 4086 times

Left click where you wan't the middle of the circle to be, then move the mouse to create the size you want. Click click "places" the circle.

d3.JPG (122.64 KiB) Viewed 4086 times

If we wanted a larger circle, we can UNDO the changes ( I'm sure you can figure that out ) and select a wider width from the top menu...

d4.JPG (123.61 KiB) Viewed 4086 times

Now I hear you ask, "why the hell did I just waste 20 seconds of my life doing this ?" . Well as I mentioned earlier, assume nothing is as it should be... While the part looks correct, its actually missing the "DOT" to denote pin 1. Yes, it has the arrow, but once the socket is soldered into place, it then becomes a lot harder to see what is actually pin 1 on the socket.. and yes, this is problem I came across with my ROM boards So I added a circle there to show easily which is pin 1...

Now a small exercise to MOVE the VALUE text to the bottom..

d5.JPG (123.57 KiB) Viewed 4086 times

At this point it's probably a good time to do a SAVE You an call the lib whatever you want. "my_lib" or "whatever_you_want" or "Library_of_doom" etc etc.

[exxos]

Next we need to actually create the schematic part.


So we click on the EDIT SYMBOL icon at the top to bring up the symbol box. Make sure it says symbol (if not click the sym button).

Type in the box as shown, I called this the "PLCC44_ROM" symbol. Then click OK.

1.JPG (114.16 KiB) Viewed 4083 times

Another pointless box.. click YES.

2.JPG (14.84 KiB) Viewed 4083 times

So we would have this screen now...

3.JPG (98.09 KiB) Viewed 4083 times

Now set up our grid. I am using lines for this part as I find it a little easier than dots for this stuff...

4.JPG (108.88 KiB) Viewed 4083 times

Now using the wire tool...

<rant>
Why is this called wire ?, shouldn't it be called line ? I guess yes its a "Wire" when we doing a wire, but in this case we are doing a LINE.. with the WIRE tool... anyway..
</rant>


Make sure layer 94 Symbols is selected in the top layer select menu.

5.JPG (108.59 KiB) Viewed 4083 times

Draw a box like shown below. Size doesn't matter exactly at this point, we will change it later as we need to using the move tool...

TIP: Left click places the line. To cancel the line tool, you can press ESC and double click after drawing your line (without moving the mouse) to cancel the tool.

6.JPG (120.72 KiB) Viewed 4083 times

At this point we should find the datasheet of the part so we know what pins we need to create..

For example I use the Atmel 4096 ROM datasheet...

AT4096.pdf

(734.75 KiB) Downloaded 162 times

I also take a screenshot as a image and have both Eagle and Pinout image side by side to make things quicker/easier.

So start placing the pins by left clicking to place them....

7.JPG (203.07 KiB) Viewed 4083 times

Select the PIN tool , and you can move and click them where you want them.

8.JPG (125.52 KiB) Viewed 4083 times

Use the MOVE tool if you need more (or less) room with you symbol.

TIP: Use F5 to move the window view about. Use the wheel on your mouse to zoom in and out.

9.JPG (123.08 KiB) Viewed 4083 times

So we should end up with something which looks like this..

TIP: Right click to "spin" the wire around where you need it..

10.JPG (138.64 KiB) Viewed 4083 times

What we have (or should have) Is 18 address pins down the left, 16 data pins on the right, 3 pins which will be CE, OE, VPP ( I spaced them away from the datapins to prevent confusion later).

Now the power pins I place at the top and bottom of the chip. Sometimes you may want a seperate power rail symbol, but that creates a whole fek-load of other steps, so I am just adding them to this symbol for now to try and keep things a simple as possible.

[exxos]

Now we need to NAME our pins using the NAME TOOL.

1.JPG (119.53 KiB) Viewed 4081 times

I start with A0...

2.JPG (13.21 KiB) Viewed 4081 times

We now have A0! Now NAME all the other pins...

TIP: Use F5 to move around and the mouse wheel to zoom in and out. Coffee or Vodka is probably a good thing to do next..

3.JPG (107.84 KiB) Viewed 4081 times

You should have something like this then..

pads-pcb.png (17.44 KiB) Viewed 4081 times

[exxos]

Now we need to link up the 2 parts we created using the EDIT DEVICE tool..

I called this part , again, "PLCC44_ROM".

Click OK...

1.JPG (123.36 KiB) Viewed 4079 times

WARNING WARNING DANGER DANGER (click yes).

2.JPG (14.16 KiB) Viewed 4079 times

Using the ADD TOOL, we need to add our part....

3.JPG (83.17 KiB) Viewed 4079 times

We should now have our part shown like this...

4.JPG (82.1 KiB) Viewed 4079 times

Click NEW at the bottom right... and select our PLCC44 package... Click OK...

5.JPG (89.27 KiB) Viewed 4079 times

Then we should see our PLCC44 package in the right window like below...

6.JPG (86.84 KiB) Viewed 4079 times

<slightly pointless note>
If we created a SMT 44 pin package, we should select it in those options and add it as a variant.
</slightly pointless note>


Make sure the PLCC44 package is selected as pointed to right red arrow...

You can double click it, or click connect at the bottom...

7.JPG (83.75 KiB) Viewed 4079 times

Then we have the connect window pop up... This is where we link our schematic pinout to the package pinout... So we need the 4096 ROM datasheet again to see what pin goes where...

Again, its useful to have both things on view on the screen at the same time...

<waffle>
In case anyone is wondering, This is the part I screwed up the STF video connector pinouts etc
</waffle>

8.JPG (152.94 KiB) Viewed 4079 times

So we look at the datasheet pinout (as shown in the right side image) and we see /CE is on pin 3 of the IC..

So we select /CE in Eagle and select pin 3... and click CONNECT...

9.JPG (135.01 KiB) Viewed 4079 times

Now our /CE pin is connected to pin 3 and shown in the right column.

(and no, I don't know what the G$1 rubbish is either )

10.JPG (59.77 KiB) Viewed 4079 times

So go through each pin one by one and connect them....

11.JPG (68.35 KiB) Viewed 4079 times

Of course there are 4 N/C pins on the ROM. So they don't connect to anything.


Click OK and Eagle will number the pins in the main window as shown below...

12.JPG (94.27 KiB) Viewed 4078 times

Next SAVE the thing.. and we are almost done...

Go back to the main Eagle control panel and click the arrow next to Libraries to expand the list..

13.JPG (71.63 KiB) Viewed 4076 times

Then look for our library name we created...

Notice the "dot" where I circled in red is smaller.. (and can be greyed out on some versions of eagle) This means the library is found but not yet loaded...

14.JPG (74.81 KiB) Viewed 4076 times

Click the dot to turn it green...

15.JPG (77.7 KiB) Viewed 4076 times

If we now create a new schematic, and click the ADD part icon, we can scroll down to find our new lib...

16.JPG (95.92 KiB) Viewed 4076 times

.. and place it in the schematic window...

17.JPG (63.09 KiB) Viewed 4076 times

Also just to show the PCB part, we can chose "SWITCH TO PCB" and we can see our PCB part also

18.JPG (89.06 KiB) Viewed 4076 times

So this concludes this epic adventure of today!

[exxos]

This took me all day to put together

I don't think I messed any steps up.. but never know

Now people know why I just wanted Rodolphe to create the libs as I had to work all this out pretty much myself

Have fun

[PaulJ]

This took me all day to put together

I don't think I messed any steps up.. but never know

Now people know why I just wanted Rodolphe to create the libs as I had to work all this out pretty much myself

Have fun

Once again thanks Exxos, Looks a little more complex than part 1 an2 but I'm going to run through it.

[exxos]

Once again thanks Exxos, Looks a little more complex than part 1 an2 but I'm going to run through it.

Yeah its a lot to take in all in one go, even more so if you take into account part 1 & 2.. We not even got into the gerber part yet, or creating our own package from scratch..

[PaulJ]

Yup, some what daunting but going to keep at it. Always wanted to be able to make a decent pc board. Lots of solutions that are wire wrapped or point to point suck. Have to get something simple made and work from there. When I retired I was going to make a dmaf2 disk controller for a couple 8" drived I picked up just for my SWTPC SS-50 computer. I really need to make a pc board since there are no more wire wrap cards for a ss-50 SWTPC buss. Thanks again exxos.

DMAF2_RedBlue.jpg (765.2 KiB) Viewed 4038 times