Hi there,
I made library of some components. I drop these components on schematics and connect them. But when I create the board the components do not appear connected. What could be wrong?
I think I made the library correctly. I made the three parts symbol, package, and device. In the device construction process I connected the pins of symbol to the pad of the package. But I am not sure what is wrong. I would appreciate your help. Thanks
Regards
Okay, putting your previous post’s aside, would you like to let us have a look at your library?
Make sure that the pins on the symbols you created are aligned to the same grid that you are using in the schematic editor. Otherwise it will cause the exact symptoms you are experiencing.
The schematic editor defaults to a 0.100" grid and I think that most symbols are built with that in mind.
:lol: :lol: :lol: :lol: :lol: :lol: :lol: :lol: :lol:FartingMonkey92:
Okay, putting your previous post’s aside
gaseous simian has feelings :lol: :lol: :lol: :lol:
.
eggfu:
Make sure that the pins on the symbols you created are aligned to the same grid that you are using in the schematic editor. Otherwise it will cause the exact symptoms you are experiencing.The schematic editor defaults to a 0.100" grid and I think that most symbols are built with that in mind.
Thanks. So as long as the package, symbol and schematics are aligned to a same grid it should be fine regardless of a specific grid, right?
.
smdFan:
gaseous simian has feelings
Lol, that’s low… Having to take comments from other peoples post’s…
Oh, and if you had actually searched these Forum’s, issues about grids/aligning in EAGLE have been covered multiple times…
eggfu:
Make sure that the pins on the symbols you created are aligned to the same grid that you are using in the schematic editor. Otherwise it will cause the exact symptoms you are experiencing.The schematic editor defaults to a 0.100" grid and I think that most symbols are built with that in mind.
Assuming we’re talking about EAGLE, yes pins of a schematic symbol -must- be on a 0.1" grid. If they are not, then they won’t actually be connected. Run ERC - it should tell you what is not connected. Don’t bother routing your board until ERC shows no errors. Inputs of a part must be connected to something. If an input can float, then in the library that pin should be I/O or passive, not input-only.
FartingMonkey92:
smdFan:
gaseous simian has feelingsLol, that’s low… Having to take comments from other peoples post’s…
Oh, and if you had actually searched these Forum’s, issues about grids/aligning in EAGLE have been covered multiple times…
FartingMonkey92 or gaseous simian,
I hope you do not take offense. Just pulling your legs 
But still I wonder, what kind of person select a name like FartingMonkey. How did you come about selecting that name? Can’t you change it to a suitable name? It is really an eye sour. May I know how old you are?
PS
FartingMonkey92,
Do you still fart 92 times a day!? :lol: :lol: :lol:
.
eggfu:
Make sure that the pins on the symbols you created are aligned to the same grid that you are using in the schematic editor. Otherwise it will cause the exact symptoms you are experiencing.The schematic editor defaults to a 0.100" grid and I think that most symbols are built with that in mind.
I did the same thing but I still have problem. The strange thing that happens is when I put two or more of the device on schematic, I notice that on the board, the GND and VCC pins are connected automatically without me making any connection on schematics. But at the same time, the pins that I connect on schematics, are not connected on the board. Thanks
If you post your library we can have a look at it.
eggfu:
If you post your library we can have a look at it.
Hi there
Since I am at work, I do not have access to the actual files. So I quickly downloaded EAGLE and quickly made two devices. In the first device I did not change anything. I put that device on schematics and everything worked well.
Then I made a second device (TEST2). This time I renamed the PINs on symbol, changed the direction of the pin. Then for package changed the name of the pad. I put these devices on schematic. It did not work. The nets wouldn’t neatly connect to pins. Then I realized that the schematic grid was different from the one I used for symbol and package. I changed the schematic grid and then it worked!!!. At home I have an older version of EAGLE 4.16 and I have been doing exactly the same thing. It just would not work. But anyhow my problem is solved now. I do not know how to upload the files here.
Everytime I change the grid to mm and my own value, then it reverts back to default. How can I change the default value of gird permanantly?
Thanks
For the schematic (and symbol in the library), DON'T switch the grid to mm. leave at .1 inches (or 100 mil). period.Everytime I change the grid to mm and my own value, then it reverts back to default. How can I change the default value of gird permanantly?
You could possibly get it to work by changing all the parts you want to use to mm grid and setting the schematic to the same grid but why bother? You will constantly be changing the symbols of every part you want to use. like it or not, don’t think metric when it comes to the schematics.
Philba:
For the schematic (and symbol in the library), DON'T switch the grid to mm. leave at .1 inches (or 100 mil). period.Everytime I change the grid to mm and my own value, then it reverts back to default. How can I change the default value of gird permanantly?
You could possibly get it to work by changing all the parts you want to use to mm grid and setting the schematic to the same grid but why bother? You will constantly be changing the symbols of every part you want to use. like it or not, don’t think metric when it comes to the schematics.
Philba,
Thanks for your advice. If you had not posted this,I would have change the gird in schematics and symbol to mm. But after your advice, I made some tests and realized your point. You saved me a lot of trouble. Thanks and happy new year.
Philba:
For the schematic (and symbol in the library), DON’T switch the grid to mm. leave at .1 inches (or 100 mil). period.
I’ve lived by this rule for a while quite happily. However I’m creating a new part in Eagle (Texas Instruments SN74CBT16233-DGGR) and the dimensions on the data sheet are in mm. This is a TSSOP-56 package.
Any advice? Is this where Eagle’s “alternate grid” comes into play? Thanks for any help.
I found my answer in the Eagle forums, and will reproduce it here for future reference.
There appear to be two approaches and this statement was eye-opening for me: “Whatever you do, there always are parts with pads that are off-grid”.
Convert mm to inches and continue as usual
Use the mm grid for the package and turn off the OFF-GRID DRC checks as soon as you use such a package. Then you must make sure to route from the off grid part to an on grid part.
Uh, nooo.
You are confusing the package with the symbol.
Never ever ever put symbol pins on anything other than a 100 mil (.1") grid.
Never ever ever draw schematics on anything other than a 100 mil grid.
Packages and boards - change the grid to suit your parts, go crazy, have a party. I will often change the grid several times when drawing a package. For example, consider a part with 4 pads in a rectangular pattern of, say, .065x.04. I will set the grid first to .065 and draw 2 pads .065 apart. Then I will change the grid to .04 and then use the copy tool to duplicate the pads and place them .04 away from the first 2. Viola, perfect alignment. I might also change the grid to draw the outline so it’s perfect as well. I wish eagle would let me define x and y grids separately.
Philba:
Uh, nooo.You are confusing the package with the symbol.
Never ever ever put symbol pins on anything other than a 100 mil (.1") grid.
Never ever ever draw schematics on anything other than a 100 mil grid.
Philba,
Thanks for the response. My understanding wasn’t at odds with what you stated, so maybe I just wasn’t clear in my post. I never meant to refer to symbols/schematics – only to package/board grids.
I think I get it now, though. Thanks a lot!