|[Search] [Contact Us]|
Eagle Power Tools
Moduli I/O USB
Moduli I/O Ethernet
Moduli A/D Ethernet
EAGLE: Various FAQ
How do I generate the component list of a circuit?
Use EXPORT PARTLIST or RUN the ULP file BOM.ULP.
Is there any software that can automatically draw a 3D image of board with components in either wireframe or rendered from the board file?
Yes, Check out Eagle3D
I'm using Eagle to create a small board that is 3" x 3". Is there any easy way to create the output files with a 3x3 grid of my little board?
Do all the following steps with a copy of your board file:
Use panelize4.ulp to copy the device names into a separate layer (so they won't be renamed there during multiplication).
Enter DISPLAY ALL and then GROUP the complete board. CUT it into the buffer, and don't forget the final mouse click to set the reference position. PASTE it as many times and where you like it.
Save the panelized board at another name.
For CAM data generation, use _tnames instead of tNames for the silkscreen file.
Alternatively, you can use GerbMerge to panelize one board multiple times, or panelize different jobs into a single board. It is a free (GPL) program.
I'm a hobbyist and want to have pads with more copper, i.e. a full pad with maybe a small centre hole for drill alignment. How do I accomplish this sort of thing?
First off if you want fully filled pads you can go to the board window and via the 'Options>Set...>Misc' menu set the 'Display Mode' option to 'No Drills' to remove the drill holes - you will see all pads are completely copper filled now. If you're wishing to have all pads nearly filled, with just a small alignment hole, use the dril-aid.ulp that comes with EAGLE. You run this and specify the drill diameter, all your pads are then done in one go. If for particular reasons you only want to do the above with some pads of a particular device on your layout, then you need to edit that library separately and use the CHANGE DIAMETER and CHANGE DRILL commands for each pad or group of pads as you wish in that device. Then UPDATE that library in your board layout to propagate your new changes
Everytime I open EAGLE, I have to size the schematic and PCB window. In this modern day and age, it should be possible for the program to save its window position and open in that position when used the next time!
In short: the window sizes and positions are saved in the project file, which is a powerful feature. Take care to have a project open when you leave EAGLE, and don't close sch/brd windows separately before.
I am a getting a message that Board and Schematic are not consistent. For some reason the new parts were not added to the schematic. What gives?
The board and shematic get out of sync if you accidently close one, and continue to work on the other. Once they are out of sync, then new parts won't be added to the board. You have two options, both might be painful.
Delete the board and redo the board from scratch. Ouch, this can be painful if it is a big board.
Carefully read the ERC file, and make the changes required to fix the outstanding differences. Use "show r27" etc. to locate the offending parts. This can be painful, if you had added a lot of parts. I have recovered a board by doing this.
The best thing is to make lots of backups -- and check the board often, to catch an mismatch early.
ALTERNATELY: As I understand layout and schematic got inconsistent because there are different nets and signals. You want to keep the position of your parts but have to re-import the net list from the schmatic into your layout. My way:
DELETE SIGNALS; in the layout
EXPORT NETSCRIPT; in the schematic
SCRIPT netscriptfile; in the layout
Yes I know, this way you lose your routed tracks, but you can keep the positions of your parts in the layout. In some cases this could be a simple way to get a consistent pair of files. Only my two cents for all those who run into such a situation. Best regards, Richard Hammerl
Look in the project directory - it is possible to rename two of the *.b#? and *.s#? files to *.brd and *.sch, respectively, to restore inconsistant files. I've done this by examining the modification times, deleting the *.brd, *.sch and *.erc files to a time before the problem happened...back up your work and only attempt this on a copy of your project. Good luck, you may save the effort of re-layout of your board!
My screen seems to get corrupted and/or I can't seem to get the text labels and component names to print out along with my schematic - What's the problem?
After running for 5-20 minutes, the display starts acting strangely (disappearing text, grey box over upper-left corner of screen, etc), and eventually, if I don't exit, it will crash.
Set the 'Options->User Interface->Always vector font' setting in your EAGLE Control Panel. This is due to some video cards having problems implementing scalable bitmap fonts - by switching to vector fonts this problem is overcome.
I recently purchased the 4 layer version of Eagle 4.09 and 2 layer layouts that were done in the free version don't seem to be allowed to have the 2 additional layers added.
A board file that comes from a Light Edition simply does not have the inner layers implemented (this is one of the restrictions of the Light Edition). You have to create these inner layers if you need them. Use the LAYER command, for example:
LAYER 2 Route2;
LAYER 15 GND;