[Search] [Contact Us]
Progettazione Elettronica Controlli di Macchine Automatiche
 |
FAQ | |
|
|
|
|
Firmware uC
Masters PCB
Circuiti Ibridi
Software Custom
|
|
B2Spice A/D
Electra Autorouter
Eagle Power Tools
SuSE Linux
|
|
Moduli I/O USB
Moduli I/O Ethernet
Moduli A/D Ethernet
LPC900 Programmer
PRM-W1 Boards
USB Key
Contatti
L'Autore
 |
Sch FAQ | Lbr FAQ | Various FAQ |  |
EAGLE: Layout FAQ
How do I flip a SMT device to the solder side?
In the board layout window, select the Mirror tool, and select the device.
How do I adjust the DRC (I'm assuming the restring settings) so I get a pad diameter of .1? Which leads me into another question: If I have pads using a fixed diameter/drill size, why do the restring values affect the size? Is there a way to turn this undesirable feature off?
The settings in the Design Rules, Restring tab affects all pads and vias. From the manual:
"...Example: The ring around a hole with 40 mil diameter is 10 mil (25%). It therefore lies in between the maximum and minimum values. If the hole is only 24 mil in diameter (e.g. for a via), the calculation yields a restring value of only 6 mil. For a board made in standard technology this is extremely fine, and cannot easily be made. It might well involve extra costs. In this case a minimum value of 10 mil is given. If you like to define a restring with a fixed width, use the same value for minimum and maximum. The value in percent has no effect in this case...."
One exception: A pad that has a higher value for the diameter defined in the library as the resulting value of the Design Rules would be, won't be changed. In this case the pre-defined diameter remains valid because EAGLE does not make the pad smaller automatically.
Why can't I zoom more?
The following snippets are from the UPDATE.TXT file in DOC directory:
Release notes for EAGLE 4.0
Screen display:
- By default the zoom factor in editor windows is limited so that the resulting virtual drawing area does not exceed the 16-bit coordinate range. This is necessary to avoid problems with graphics drivers that are not 32-bit proof. If the graphics driver on a particular system can handle coordinates that exceeed the 16-bit range, "Options/User interface/Limit zoom factor" can be switched off allow larger zoom factors.
Release notes for EAGLE 4.01
Bugfixes:
- Fixed not limiting the zoom factor for small drawings.
I have found that the smaller the board, the greater you can zoom-in with options/User interface/Limit zoom factor switched on. If your graphic card is 32-bit enabled, try turning this switch off. If has you zoom-in and the display starts to look funny, then your graphic driver isn't 32-bits and you should turn the switch back on and live with the limited zooming ability (or look for a 32-bit driver for your G-card)
Can I have different trace widths?
Yes, go to EDIT:NET CLASSES and you can set up default widths and clearances for various nets. Then in your schematic, go to CHANGE:NET CLASS and change the type of each track. Your autorouter will use these settings to autoroute wires, and DRC checking will use the settings also to check for clearances and width problems.
How do you cope with different board outlines?
My approach to this is to create a custom library of PC Cards as components. Draw the PC board outline with mounting holes and other details as a PACKAGE. For the schematic half of this "Device" I just use text on the symbol layer that says something like "using PCB #12345". That way this text shows up on the schematic for documentation purposes. NOTE: I even include dimensioning info for the dimension gerber in the "PACKAGE". This has the added advantage that you can NOT accidentally move a PCB edge dimension line or mounting hole during the PCB layout process.
How can I place a ground plane in my circuit?
Type "poly gnd" and draw a polygon around your board. Then press the RATSNEST button - hey presto! You can turn this off by typing "set polygon_ratsnest off" or just "set polygon_r off".
Is there a way to enlarge the pad size of ALL the resistors/capacitors without going through each one individually?
Under DRC -> Restring tab -> Set PAD percentage higher
Could somebody explain what to expect when diameter = auto in a via?
The outer diameter is calculated automatically based on drill diameter and the "restring" setting in the DRC parameters. The same applies to pads in packages of which the diameter has been set to "auto".
How do I delete a via connected to power? When I try to delete it the PCB program gives a message stating that the operation must be done in the schematic. I don't see the via in the schematic so I cannot delete it.
Use ripup to delete it. Delete will try to delete the whole signal.
How do I add a PLCC socket on my board (namely the S44)? I tried adding it using the add command but it says: "can't backannotate this operation. Please do this in the schematic". But this socket isn't available in the schematic section since the sockets are a package-only library. What do I do?
Add the socket as a package to the library that contains the IC in question (if it's not already there), and add it as a package variant for the specific device (if it's not already there). Then you can use CHANGE PACKAGE to swap between direct soldering and socket.
What does "99.5% finished in Autorouter" mean? If it means 0.5% left, how can I find the unrouted wires?
Use the RATSNEST command and in the info bar there should appear a message like:
5 airwires left
Then, display layer 19 (unrouted). You should now see the unrouted wires. If everything is routed RATSNEST displays "Nothing to do" in the info bar. Another way to find airwires is to select ROUTE and click on the board. The closest airwire will be attached to the cursor with a trace. You can then zoom into the area were the trace is being placed. If you don't want to actually place the trace after finding the airwire, push ESC to abort the ROUTE command.
I have a complex schematic that I want to autoroute, but it leaves too many unrouted tracks. My question is: how do I start a new autoroute? Playing with options/parameters doesn't give any better results? What can I do to start auto route without all this mess? What are the differences in the direction signs? "/ \ . |"
Use the Group tool to select all the traces in the board view, then use the Ripup tool, but RIGHT click the board, all the traces should revert to air-wires. Also reroute with the Routing Grid set to 10 (I think the default is 50, and that is usually too big). [David]
To delete an existing route, use RIPUP ALL. Autorouting in general is a complicated subject, and the Eagle manual contains a reasonable bit of information on it. You really do need to read the manual. The autorouter is not intended to be an "idiot proof" feature.
If you have too many unroutable traces, then you may need to reduce the track width closer to the PC house limit and make the routing grid finer. However, you can only throw so much brute force at it before the results will taper off. In the end a good layout is the most important single factor. If you've done all the right things and it's still not routable, then consider adding a layer or two (For example, there is no point to a 3 layer board. The board house will probably use a 4 layer process and charge you accordingly anyway.) [Olin]
Before reducing the dimension of the traces, you might try to change the directional organization of the routing. There are two menus (left up) with TOP and BOTTOM preferred direction. Choose the star and see how much it helps. Then start decreasing the number 50. Go to 30, 20 and below in steps of one... DO not choose a parameter too small (5 or 8) otherwise traces are too thin and close each other. [Stefano]
There are times when the airwire connection generated by the ratsnest command are not ideal (from an electrical point of view. Unfortunately, the program doesn't seem to like it if I route the connection by a different route. Is there any way to force the airwire to move to a different connection?
Here's a "trick" I often use when hand routing. Route the airwire from the component end, near to a trace you want to "T" into, but stop short. Use the grid so you know where to do what comes next. In line with the end of the trace you just left dangling, use the "split" command, and click on the trace you want to T into. Do another ratsnest command and behold the airware from the end of your dangling trace should jump to the split you just made, provided it's closer to the split than any other "vertex" of that net.
I'm new to Eagle and need some guidance on Gerber file creation.
Try this link: http://www.precma.com/informatica/tutorial.htm or http://www.precma.it/informatica/tutorial.htm
Brd FAQ
|
Sch FAQ | Lbr FAQ | Various FAQ | |
Site made with Sworg - Simple Web Organizer
 |
All Rights Reserved - Copyright Notice |
 |