Hi, i’m designing a prototype for a SIM548 module, in which i use two MAX232 i.c. for level shift the four serial ports of this module. But when i’m putting the capacitors for the MAX232’s something weird happens to me:
the two capacitors which go on pins 1,2 and 4,5 appears good, and the cap between the pin 2 and pin 16 between pin 2 and Vcc appears good too…
after that i placed a cap between pin 6(V-) and GND, and in the shematic looks good, but when i get a board this connection airwire doesn’t appear, everything looks OK but this cap appears with the ground connection but not the connection to the pin 6 in both ICs.
Do you have a idea about what can be happening? The part i’m using is the Sparkfun Library’s MAX232PTH, is a problem with the lib or is my fault?
Only things I can think of are fairly far reaching. You’ve tried hitting ratsnest a couple times to see if it figures itself out? Grab the parts and move them around in the schematic to make sure the nets are actually attached to the part.
Sometimes it’s looked funny to me if I’m in a signal polygon, I don’t need to route a pin, since it’s already attached to the polygon. I would think this would be more likely if it was ground and as soon as you hit ratsnest the polygon would have filled and it would have been obvious.
I’m no Eagle guru, I’m sure someone else might have a better idea.
rcarvajal:
Hi, i’m designing a prototype for a SIM548 module, in which i use two MAX232 i.c. for level shift the four serial ports of this module. But when i’m putting the capacitors for the MAX232’s something weird happens to me:
the two capacitors which go on pins 1,2 and 4,5 appears good, and the cap between the pin 2 and pin 16 between pin 2 and Vcc appears good too…
after that i placed a cap between pin 6(V-) and GND, and in the shematic looks good, but when i get a board this connection airwire doesn’t appear, everything looks OK but this cap appears with the ground connection but not the connection to the pin 6 in both ICs.
Do you have a idea about what can be happening? The part i’m using is the Sparkfun Library’s MAX232PTH, is a problem with the lib or is my fault?
As someone else said, run ERC. It could be that your problem cap is not really connected.
ok, looks like the ERC gave me some hints about this. It says two warnings regarding to my problem:
Net N$11 overlaps pin.
Only one pin on net N$11.
This clearly says that the net is wrong. I tried to redo the connection in both ways, from ic to cap, and from cap to ic, i’ve never changed the grid size from 0.1 inch in the shematic view.
I’m still confused about if it is a lib problem or my fault.
Any ideas?
EDIT: Great!!! I solved my problem… it was a strange behavior in the grid anchor, when i released the net on the ic. pin the wire ended up far away from the pin. The ERC gave me the hint. Thanks for your help.
Try this - delete the cap and then replace it. Using net - start FROM the cap and connect it to the other pin. Run ERC and see what it says. Eagle is notoriously fussy about where it sees the mouse. You might want to zoom in a bit more when doing the net so you are absolutely certain it’s doing what you meant. It’s not unusual in Eagle to overshoot the pin and not make an actual connection even though the schematic shows the the pin and net as connected. A pin is a single point - it you don’t hit it within 1/2 a grid distance, it won’t connect. Eagle really should make a positive feedback mechanism to let you know when you are on an “active” point.
In general, use the validation tools available to you. When you get to the board design, don’t forget DRC.
I HAVE run into this and I don’t know if it’s a minor bug or possibly the way I place parts sometimes. I have made it a habit whenever I add in a part like you did to take the move tool, grab the part and then “pull” it away and see if the net stays connected to it. If not, I delete the part and try again. Sometimes, I will stick a connection “dot” at that point and that will force a connection. Of course and ERC check helps verify this and a quick check of the board for an airwire does as well.
rpcelectronics:
I HAVE run into this and I don’t know if it’s a minor bug or possibly the way I place parts sometimes. I have made it a habit whenever I add in a part like you did to take the move tool, grab the part and then “pull” it away and see if the net stays connected to it. If not, I delete the part and try again. Sometimes, I will stick a connection “dot” at that point and that will force a connection. Of course and ERC check helps verify this and a quick check of the board for an airwire does as well.
Yeah, I use all of those, too. Kind of crude but effective. I’d love it if, in the schematic, you could have each pin have one of two colors - red: not connected; green: connected. That way, you get instant visual feedback when a connection is made.
With Pulsonix, the cursor changes to an ‘F’ (for Finish) when close to a pin; a single click and the connection is made making it practically impossible to make a mistake and miss a connection. Someone should suggest it for incorporation into Eagle.
Other packages have something that completes the connections automatically if a part is changed, it’s often called “autoweld”. Again, someone should request it.
gussy:
The problem is when you delete a part, then place a new on in its place, and expect the wires to join up. I get this all the time like the others.
Easy way I fix it is grab the end of the wire, put is somewhere else then move it back to make the connection.
If in doubt, re-route!
there’s a much easier way to reconnect the nets. (re)place the chip. then using the select tool, select the chip (ie. click on it’s origin). That’s it. All pins are reconnected (if a given pin and net share the same coords). You can see this by selecting and trying to move the part. Don’t know if that’s deliberate or not but it’s very convenient.
