PRECMA S.r.l. -

[Search] [Contact Us]

Progettazione Elettronica Controlli di Macchine Automatiche

FAQ

PROGETTAZIONE

Hardware
Firmware uC
Masters PCB
Circuiti Ibridi
Software Custom

SOFTWARE

Eagle CAD
B2Spice A/D
Electra Autorouter
Eagle Power Tools
SuSE Linux

PRODOTTI

Embedded Linux Board
Moduli I/O USB
Moduli I/O Ethernet
Moduli A/D Ethernet
LPC900 Programmer
PRM-W1 Boards
USB Key

Cerca nel sito

Contatti

L'Autore

Brd FAQ

Lbr FAQ

EAGLE: Schematic FAQ

Where are ordinary resistors?
They are in the rcl library -- this is the resistor-capacitor-inductor library.

How come my wires do not connect reliably?
You should use the Net tool for wires in a schematic, and ... It is due to your non standard grid settings (or the component being created on a non-standard grid) - the pad must be exactly on a grid traversal for connection. Look at the user language programs called cmd_snap_board.ulp and cmd_snap_schematic.ulp to help get your components to all line up properly.

Since the loading time of the "add" command is too long for my system, I want to disable some libraries in control panel. However, if I restart Eagle, all libraries will become enabled again. How can I solve this problem?
The information on which libraries are in use is stored in the current project file. If there is no project loaded, the information won't be saved.

Can one copy gates? Or must I always go fetch a ground gate every time I want to ground a net? Copying a gate yields a warning that I cannot copy gates.
NOTE: More recent versions of Eagle do let you copy gates using the COPY tool. Otherwise, click GROUP (dotted square), surround the gate(s) with LEFT MOUSE BUTTON clicked. Click CUT (scissors symbol) and use RIGHT MOUSE BUTTON on item(s). Then click with LEFT mouse button on PASTE, and place the component. This also works to copy stuff from one library to another, although it is slow as you have to close and open libraries.

How can I connect the implicit power pins?
If you choose the supply parts with the appropiate SUPPLY parts (e.g., VCC, GND), then your parts will connect automatically, and you will be able to see airwires on the board. Alternately, you can INVOKE the part; a popup will let you add the supply pins to the schematic.

If I have INPUT pins on an IC, but I don't want to connect it, how can I eliminate the message error "unconnected INPUT Pin"?
By convention, INPUT pins must be connected. If you have pins that can be optionally used but also left open, you should set them as PASSIVE. You need to do this is the library editor. Use the Change->Direction->pas to change the pins that you want to be passive.

How do I split an existing schematic so that I can have it on two seperate sheets?

Make copies of schematic and board (for safety).
Close the board - annotation is turned off by this.
Select a group you want to move to another sheet, and CUT it.
Delete the group (right mouse key).
Load the board again (schematic still loaded).
Select the target sheet and PASTE the group there.
Run ERC to regain annotation. Normally, schematic and board should be consistent again.

How can I have a small grid for better placement, but fewer lines?
I never realized the usefulness of this option, but it helped in this case. As stated above, I found it a nuisance to have to keep switching the board GRID spacing from 0.05mils to 0.01 mils (back & forth), just to "align" parts badly placed by the editor. Well, I found that if I set (or leave the default) value of spacing at 50 mils, but changed the MULTIPLE to 2, I end up viewing a normal 0.10 inch spaced grid (twice 0.05), but with active and mouse "reachable" 0.05 inch grid positions (which have invisible grid lines). Now I can more easily shift the placed parts onto the 100 mil through-hole grid from the odd 50 mil placement - without the need to keep switching back to the GRID command each time. And, as the actual 50 mil spacing is invisible, in this case, it is less confusing to view and work with. Since the project uses 0.1 in components exclusively, I think I will set the Grid MULTIPLE to 2 in the Eagle startup file. That is a more appropriate "standard" default.

How do you renumber a bunch of sheets at once?
I agree being able to renumber sheets would be a "very-good-thing"!, here is my work-around. When I have completed the schematic...
Add as many new sheets as there will be in the finished schematic.

Close the PCB file for the duration (this is the ONLY time I work on a schematic file with annotation deliberately disabled!)
Find what you want to be the last sheet of the schematic. Turn on all layers group, cut everything using the lower left corner (0,0) as the insert point (helps to have the grid set fairly coarse, ideally at .1" --Delete the group you just defined and cut
Move to what is now the last page in the project.
Paste at point (0,0) REMOVE the now empty sheet.
Repeat the above steps until all sheets have been cut-pasted into the correct order.
Open the board file and run ERC to make sure you haven't lost consistency.

It would be REALLY useful to have notes on a schematic
Here is the workaround I have used. I create a component called "NOTE" which only has a >NAME and a >VALUE. I then add a number of NOTE parts to my drawing, and for the part name I call them 1, 2, 3, 4, etc. (Note there is no letter in front of the number. This seems to work.) Then I add text by the component, "See note 1". Note 1 says R1 is a 10 watt wirewound by Gymcrack Corp or whatever. The cool thing is that NOTE 1 SHOWS UP IN THE BOM when I export a BOM using BOM.ULP. So it is really easy to add a note to your component BOM list. A couple of suggestions:

Put your "NOTES" on a layer which you leave undisplayed when printing the schematic.
Make the "NOTES" text a really really tiny font.

PRECMA S.r.l.

Brd FAQ

Lbr FAQ

Site made with Sworg - Simple Web Organizer