Qs re EAGLE use

Q #1: Board layout: OK, i laboriously* created the package outline i needed and placed four of the parts on a board in one line. Wiring is added. Now for efficiency i would like to copy that set of parts and place in a line above. Then copy that set of 4 to a line above, then copy that set of 8 to a line above, then that set of 16 to a line above, and then that set of 32 to a line above. HOW? "group" is useless - unless there is some magic needed.

Then the whole mess needs to be copied and placed on the back side. HOW?

I will then edit each side as i see fit (some of the resulting parts will be deleted and other parts will go in their place).

The copy-a-group trick will save a whole lot of time.

• Eagle is crappy; have a nice looking picture of a package layout and want to change the SMT pad, select change, click on pad and the part PIN gets changed as well as rotated (crappy, crappy). Found a partial work-around by making one of the high numbered layers invisible, making desired changes but damn pad gets rotated on resize. So i said F* it and changed sizes then went back and rotated each one to where they should have STAYED (crappy, crappy). When done, made that layer visible and all was OK. And this was after i "upgraded" from 5.0 to 5.11 the most recent version that works in Win2K.

Q #2: Creating a new package in the library problem: I start with a package close to what i want, and after a lot of fiddling (see comment about crappy in note above) i get what i want to use. Now i foolishly renamed what i had and changed the description (since what i now had WAS different, this seemed the logical thing to do). Save and exit. CRAPPY! The original part that i had used for a model IS GONE! Damn good thing i backed up that lib file as a different name. SO.. HOW in the F do i either copy or move this new package into the original lib file without messing up any other package in that file?

"Robert Baer" schreef in bericht news:zJWdnbZJs_wqLfvSnZ2dnUVZ snipped-for-privacy@posted.localnet...

As for Q1 I don't know.

Making a new package out of an existing one, you start to make a copy of it and give that copy the new name. Then change whatever you want to in the copy and save it. Which all can be done in the existing library. You have to update the library to make the new package available. Connect the package to the component, save all and update once more. I've done this tens of times as I often want larger pads and a smaller holes.

petrus bitbyter

o a

Hi Robert, I use Eagle a little. I think a group, cut and then paste will work. The cut command is a little 'weird', but it doesn't really cut it just copies.....

The only issue is that this will trash the schematic! But maybe you don't care about that?

Yeah flipping and rotating a 'group' of objects is not always well defined.

ts

ers

e.

nce

Hmm, yeah you need the same group/ 'cut' trick. Group, and 'cut' the package you want to mod. Then start a new package (new name) and paste in the package you will change.

in eagle 'cut' =3D 'copy'.

George H.

ed

ace

to a

supposedly theres a way to do it in the latest version, but it is possible with a bit of work in old versions too.

here goes:

draw schematic and, draw pcb and route the group of parts

Close schematic editor

cut-n-paste group of parts and routing as many time you need in the pcb

fix names of gnd and supplies, they will get names like vcc1,vcc2 etc.. instead of just vcc

open schematic editor

cut-n-paste same group of parts same number of times

run erc, fix anything you missed

-Lasse

aced

place

Thanks Lasse, I'll try that if I ever have the need.

George H.

I used Eagle for over 10 years and have to confess that I like the package but did take time getting used to its idiosyncrasies. Took some work but I was really happy with it after a couple of layouts

The big issue with eagle is CUT actually means COPY.

so you need to group/cut/ paste to get a copy done.

Where eagle excels is synchronisation between sch and brd, but to do what you want you need to break that.

There are also ULPs that do pretty much exactly what you want - have a look here

how about changing pad dimension so instead of [x y] you use [y x] would that work? not really clear what the problem is.

open the lbr you want to add a package to, then in the lib browser you can right click a package and select add to lbr. This copies an existing package into your open lbr ( I think - don't have Eagle on this laptop)

Or you do the group/CUT/paste routine - not intuitive but it does work.

open package you want - do the group/cut part. make/name a new package and paste.

Thank you very much for the forum reference. I could make some rather useful suggestions that everybody would love to have..for example, one normally draws a schematic the way one would lay out a board..but Eagle destroys all of that physical relationship and "randomly" scatters parts by the board and one has to laboriously move all the damn parts..furthermore a number of the wires at times are connected wrong and are an extreme bitch to correct. One would think that after all of these years that SOMEONE would have bitched loudly, asking for a pre-layout placement based on the schematic (or selected area). There are a heck of a lot of users a LOT less stupid than i am, which would guarantee such complaints. Leading to the conclusion that those complaints were ignored.

Well, i think i almost did that - except "make a copy" first, which i do not know how to do. The Rename changes the original component in the lib, thereby screwing up any possibility of keeping the original - unless one quits and aggressively NOT save. The net result of that is exactly as if you did nothing!

WRT Q#2: Just tried "group..cut..make new package with new name..get empty work area(looks good so far)..paste" and got error message "paste buffer is empty". Did not even bother to save..i quit while i was ahead.

WRT Q#1: Just tried "group..cut..paste" and got error message "paste buffer is empty". So, being stupid, uninformed and an idiot, i tried "group..cut..copy" and then tried to"grab the highlighted group for (at least) moving and got only the one part at the cursor = = NO group!

• This is where it is a bit difficult if not possible to follow,because i made no schematic. I think all i have is just a package drawing after buggering and destroying the original package.

Sounds like a way to do what i want is to start with a schematic and expand there. Naturally, when i go to "make a PCB" the parts will be all over the place and NOT with placement i carefully gave. Cannot "win".

• BUT..the error message eXplicitly stated that the paste buffer is empty, so it is still useless.

• Tiz "broken" in there ain't no schematic (yet). Am too stupid to make a PCB outline - but at this preliminary point that is a trivial concern.

• Problem was, the device PIN got changed and NOT the pad..never mind i eXplicitly put the cursor right on the pad. crappy. Second problem was after making the pins invisible, the damn pads rotated on resize...i DID NOT ASK FOR THAT!!!! crappy.

• Dunno how one could interchange X an Y and at this point it does not matter because i have a package the way i want it.

• Maybe i am doing this all RONNGG. 1) "Launch" Eagle. 2) Select randumb project. 3) Select a board and get that window. 4) Click "library"..open..select one of them. 5) Now have a new window, a library window (empty at present). 6) Click on package i want..as that seems all i can do ..and this gives me a "filled" window where i could alter the package,but...but....if saved, the ORIGINAL package is destroyed and one has a new package - - NO GROUP/CUT/PASTE possible as paste buffer is empty.

Group/Cut Paste definitely works on Eagle. After you have made the selection with "GROUP", type in "CUT" and click on the area by using the the right side mouse button. All group actions require the right mouse button, the left one is for single objects.

The way of duplicating PCB and SCH groups is something awkward, but should be better now on the actual version. Unfortunately, I have not tried it yet. The old-fashioned way is done via Group/cut and Paste. Close the PCB, do the Cut/Paste thing on the schematic only. Save the Schematic, close the schematic. Opent the PCB, do the Cut/paste thing, save the PCB. Then open the Schematic again. Repair Vcc1 vcc2 to Vcc and so on. Only a few signals go corrupted.

A reasonable placement of parts after creating a schematic is not implemented, as you noticed already!

Regards Tobias

p.s.: I have been using Eagle since Version 1.0 and switched over to Altium at the beginning of the year. I can tell you that I encounter the same obstacles now as you do!

laced

place

f 8 to a

One thing I like about eagle is it keeps the pcb and schematic in 'lock step' agreement. You are not allowed to make changes to one without changing the other. What you are trying to do breaks that rule... and you have to undo the damage once you are done... bit of a PITA, but I really like the enforcement.. otherwise you tend to get lazy. (Maybe its a German thing.)

nd

No that will make it worse. In fact in my version of eagle (4.15) it won't allow you to add parts to the pcb only to the schematic.

Yup added parts fall outside the pcb outline. That's kinda nice when adding parts to an existing board. But something closer to the schematic would be nice too. Here's a trick I use when moving parts on the pcb. With the movment tool selected, if you type the name of a part into the command line (R32 for instance) that part appears at the mouse pointer. So if you have the schematic next to you, you type in the wanted names and slap them down near where you want them. (Saves scrolling the window all over the place.)

George H.

IN

to

on

ng

al

y.

Hmmm, Can you make the group-cut-paste commands work on just the pcb?

George H.

aced

place

side.

parts

IN

layers

to

nt

use.

(since

is

py"

in versions before 6 you need to do group, cut, and then hit the green traffic light, status bar will something like "hit go to select group"

in version 6+ you group, copy, right click and theres a "select group"

-Lasse

IN 6.01 it is Group. right click in selection and select copy group. I think that this may have changed since 5.11. I don't see a cut in this version.

some permutation of this will work, but the order is important e.g. select group icon group the parts select copy icon right click in group move and left click where you want it.

don't need any of eth above - other than launch eagle

OK

now in the control panel expand a lbr containing a package that you want. Right click and selct copy to lbr

Well, open the library you want to work with and issue the command:

copy package_you_want_to_copy.pac@library_where_that_package_resides.lbr name_of_new_package

You have the copy right at your hands and can modify whatever you want without effecting the original. When you're done you have to save, update and connect the new package to the component. Update once more when you want to use the package.

petrus bitbyter

ur

n a

PIN

to

ion

ld

ing

nal

ng

pty.

Geesh, why can't software have less changes over time? Refine rather than expand. I'm using version 4.15 so any advice may be useless. George H.

with "GROUP", type in "CUT" and click on the area by using the the right side mouse button.

objects.

better now on the actual version. Unfortunately, I have not tried it yet.

Cut/Paste thing on the schematic only. Save the Schematic, close the schematic. Opent the PCB, do the Cut/paste thing, save the PCB. Then open the Schematic again. Repair Vcc1 vcc2 to Vcc and so on. Only a few signals go corrupted.

as you noticed already!

the beginning of the year. I can tell you that I encounter the same obstacles now as you do! BINGO! The SECRET (shh..do not want anyone to know) is "All group actions require the right mouse button" with emm-faa-sys on the word RIGHT. THANKS!!! Still do not have a schematic for this board,but do not care (yet). Stupid,stupid,dummmmb question - - WHY has nobody since Eagle 1 or 2 (ie all these years) ever complained / asked for / demanded reasonable part placement based on the schematic?