eagle datasheet

[nabilhattaz]

hi,

anybody know any links or web page to download eagle library. i am using the eagle software, but the thing is, the components and parts that i am looking for use is not in the library. so any body here can show me where to download the parts or components or teach me to build the components myself.

thank you very much.

 

[mneary]

Have you downloaded the entire set of libraries from cadsoft?

If so, and your part isn't there, then go through the tutorial. I fount that it is excellent, and after an hour I was making my own parts.

 

[3v0]

More then half the trick if knowing what libs the components live in.

What components do you need?

 

[jpanhalt]

My policy is to download from the Cadsoft site libraries that look reliable. That is an unsubstantiated prejudice, but I trust something from Cadsoft more than something from an unknown individual. Then, I make my own components using the packages and symbols that are most relevant in the packaged libraries.

Do it a few times and you will get over the activation barrier for doing it more. It really is not hard; it is just not Windows. For example, today I wanted to use an SO-8 version of the LM7805 voltage regulator. I searched Cadsoft, didn't find it, and built it from and SO-8 package and and a 3 terminal version by just adding the additional pins to the symbol. John

 

[nabilhattaz]

well some of the components is really hard to find. im looking for max485, irl510. and some other components still looking for it. is it hard to build the components by myself?

 

[3v0]

well some of the components is really hard to find. im looking for max485, irl510. and some other components still looking for it. is it hard to build the components by myself?

You did not say what package you were using.

If you look at the data sheet you will see that the following share the same pinout in an 8 pin package. pinouts differ between packages but are the same between the devices.
MAX481/MAX483/
MAX485/MAX487/
MAX1487

The maxim library shipped with eagle has the dip package MAX481CPA, the SOIC package MAX481CSA, and the uMAX package MAX481CUA.

It would be easy enough to make a copy of the MAX481xxx with a new name. Of if you want to cheat just use the actual part name as the NAME and/or VALUE. Be careful not to become confused.

If it comes down to making you own parts start with the parts datasheet. Do the tutorial on making parts!

 

[jpanhalt]

well some of the components is really hard to find. im looking for max485, irl510. and some other components still looking for it. is it hard to build the components by myself?

The IRF510 is there under "transistor-fet."

As mentioned, the MAX481 is there under "maxim." Place that component on your schematic. There is no need to remember what the real component is, or need to make a copy.

After it is placed, click on the component "value" button. You will get a warning message that the component has no user defined values. Click that you want to change it anyway. The name MAX481XX will come up in a dialog. Change the name to whatever you want it to be, click OK and you are done. It is no different than using a passive component, except for the warning screen.

John

 

[Boncuk]

Eagle

Hi all,

Eagle uses good libraries, fairly good libraries and junk libraries.

I've been working with Eagle starting out at version 2.5.

Here are the steps for those who don't know exactly how to add a new component to a library or make a new library.

Let's start with a package: the same packages are used for many coponents. You can skip making a new package selecting the one you want to use (even if it requires small changes like the shape of the body or additional pins). Open the library with the package you want to use: Group the entire package including the text >NAME and >VALUE. Then copy it to the paste buffer by using the scissors symbol and then hit the button next to the green traffic light symbol. Now the package is in the paste buffer. Open the library you want to put the package into. Click package -> New and type the name of the package, e.g. SOT23 (If it's already there use a suffix like SOT23-1) Then paste the package onto the screen. Make your necessary changes and save it.

The symbol should fit easily into the schematic so you should know where to connect what to avoid crossover nets, which become confusing the more there are. Create a new symbol like you did with the package. Give it a name which refers to the function as well as to your specific schematic you are planning (e.g. NE555 for general purpose, NE555-P for PWM applications and so forth). Since you will type the pin names already into the symbol you should CHANGE -> Visible -> PAD (Activating BOTH gets too confusing).
Number the pins with the pad numbers and save the symbol.

Creating a device is the last necessary step. Click DEVICE -> NEW and type in the device name e.g. IRF450. Click ADD and select the symbol you've created before. Give it a name like IC or U for an integrated circuit or Q for transistor (Germans use T for transistor). Place the symbol close to the zero-zero point (X and Y position) because it will be referenced to that in the layout. (Having the reference point miles away you will hardly be able to move that part, in the worst case the reference point will be off the PCB. You can force that situation and then create a board. Click WINDOW-FIT and everything is fitted into the window, including your reference point, causing a small PCB on the screen) Finally click CONNECT and connect the pins and pads properly. If you are unsure about what to be connected just connect one pair of pin and pad, then click OK. The display shows what you've connected. If it's OK go to the next one, if not, click disconnect after you selected the faulty connection.

I hope this advise is good for newcomers on Eagle, and yes, Eagle is still DOS-based. If there are any questions arising making libraries of your own I'll be glad to help you, even "constructing" a new part which is not to be found in any library. Just email me the data sheet and you'll get the desired part with a package of no more than 1/1000mm tolerance.

Regards to all

Hans

 

[jpanhalt]

Here is a hint and a suggestion.

Hint: You can create a device without a package. For example, I created a device called, LINKNAME. It is simply a name inside a narrow banner (copied from the Supply2.lbr). How do I use it? When I need to place components on the schematic that will eventually be off-board, such as a switch, I connect the pins on the switch to LINKNAME, label each net appropriately, and place it wherever I want to. Then when I make the board, I can drop that component (there is no package, so LINKNAME doesn't show), but the connections to headers and other connectors remain intact. There may be a better way of doing that, but I find it useful. It avoids having to draw connections all over the schematic to the off-board components. You can also use it to connect the pins of headers without having to draw a line to the actual connection point in the circuit.

Suggestion: Since I joined this forum there have been many useful suggestions and hints on using Eagle, but they can be hard to find mixed in with the rest of the posts. Perhaps the moderators would consider a separate heading under Electronic Content called something like, Schematic Capture/Board Design Software.

John

 

[nabilhattaz]

Thank you all, for all the advices and infos given. it really helps me a lot since i am new to this software. Thx again.

 

[shimniok]

I realize this is really old, but thought I'd also point out in case it helps someone else, you can create a package that consists only of wire pads. Call it "OFFBOARD" or something similarly descriptive.