Eagle users look this way....

[Papa_lazerous]

Just started using Eagle for my schems and layouts and although the learnign curve is a little steep at first I have a feel for it.

There is one area that I am in the dark about and advice would be appreciated.  Say for example I have drawn the Schem and then I produced a pcb layout and then I notice an error on the schematic.  If I change the component or the text associated with it what do I need to do to make this update on the pcb?  Is it a case of hitting refresh/redraw which I think is F2 or do I have to click something for it to update it

I am using gaussmarkov's library so a big thanks to him for putting in the ahrd work up front, anyone else who has a library of useful pedal builders parts or IC's that we might use feel free to bombard me with them 

Thanks
John

[Baktown]

I can't seem to get Eagle to install on my laptop.  I copied all the zipped files, and uncompressed them, but I can't find an installation file anywhere.

Is Eagle designed to be run in AutoCad?

Axl Bundy

[Papa_lazerous]

this link is the download for the installer ftp://ftp.cadsoft.de/eagle/program/4.16r2/eagle-win-eng-4.16r2.exe  you dont need to extract any zip files it just installs straight from the desktop

[qwixzh]

I can't seem to get Eagle to install on my laptop.  I copied all the zipped files, and uncompressed them, but I can't find an installation file anywhere.

Is Eagle designed to be run in AutoCad?

Axl Bundy

have you used this file?

ftp://ftp.cadsoft.de/eagle/program/4.16r2/eagle-win-eng-4.16r2.exe

[Papa_lazerous]

lol I beat you to it

[qwixzh]

There is one area that I am in the dark about and advice would be appreciated.  Say for example I have drawn the Schem and then I produced a pcb layout and then I notice an error on the schematic.  If I change the component or the text associated with it what do I need to do to make this update on the pcb?  Is it a case of hitting refresh/redraw which I think is F2 or do I have to click something for it to update it

after updating your schematics, just go to the pcb layout and you'll see the new part, although not in the position of the original part you replaced.

hope this some how helps.  

[qwixzh]

lol I beat you to it

haha yup! you got me! 

[Papa_lazerous]

Thanks I will try again later or at some point over the weekend as I have lady company, ladies and schematics dont mix, and to be honest boobies win everytime

[Auke Haarsma]

we need pics to verify that statement!

And qwixzh is right: just update the schematic (make sure you have both windows open, pcb and schematic). If you remove a part from the schematic, it will be removed from the pcb.

[Papa_lazerous]

What exactly do you want verified with pics?  I think I could land me a ban from the site if you require anything unsavoury and I kinda like it here

[Dave_B]

As long as she's not holding up a Z-Vex schematic you should be ok.   

[gaussmarkov]

just to add some detail:  a new component on the schematic appears off to the left of the layout area, just as the components appear when first making a layout from the schem.  if the unrouted layer is visible (turn it on with "display unrouted" or an abbreviation of same), then you will see the so-called rubberband connections shooting off to the left of the pcb layout area where the component is sitting waiting to be placed.  if you remember the name of the new component (say it's R5), then you can type "move R5" and -- bang -- it will appear as your cursor and you can drop it where you like.  if your cursor is not over the layout, it will still be off screen.  but as soon as you bring your cursor over the layout you will see it.

I am using gaussmarkov's library so a big thanks to him for putting in the ahrd work up front, anyone else who has a library of useful pedal builders parts or IC's that we might use feel free to bombard me with them 

i'm pleased that you have found that useful.  by the way, i am open to suggestions for improvements or addititions.

all the best, gm

[Papa_lazerous]

As long as she's not holding up a Z-Vex schematic you should be ok.   

So the schematic I have of a fuzz factory should be out of shot then lol...... I built one a while back and I didnt like it.  I may have actually bought one if I did.  But it was a little too lively for me lol

[Papa_lazerous]

Thanks Gauss your article was really helpful to me, it certainly cleared up the isues with finding stuff on the library

Steep learnign curve but worth it.....  Only thing though I havent got to yet when I want to print onto Press and Peel what do I have to do to export just the tracks to the printer and at the correct scale?  I have seen nothing on this

[gaussmarkov]

i have figured out two ways to make pcb images.  one produces PNG files and the other EPS, which i prefer because they contain vector graphics.  here's an outline of each method.

to make a PNG file for PnP, you can use the EXPORT command.  i put all the commands that i use in an eagle SCRIPT file and execute that from the command line in the layout editor.  but it's not that much to type.  you can mouse click your way through these commands also.  type each of these lines into the command line:

Code Select Expand


set palette white;
display none bottom pad via;
export image yourpcb.png monochrome 300;


the SET PALETTE command ensures that the traces and pads will be black and the rest of the board will be white.  the DISPLAY command turns off the display of everything (NONE) and then turns back on the BOTTOM, PAD, and VIA layers that are in your layout.  i have seen some people use the TOP layer for their traces, and if you do this you will have to display the top layer.  but this is an unconventional practice.  i suggest using the BOTTOM layer if you want to share your work with others.  the EXPORT command creates a PNG file that is black and white at 300dpi.  you can make other graphics file types if you prefer, just change the filename extension.  you can also use a higher resolution if you prefer.

if you import the file produced by the EXPORT command into a wordprocessing program, then you should be able to print it out correctly.  just don't resize the image.

the second method is to use the CAM Processor in eagle.  it's under the File menu in both the schematic and layout editors.  save your work first, then open up the CAM processor.  now,

• in the Device dialog choose EPS, or whatever you prefer
• click on the File button, and specify a location and name for your output file
• in the Style section, uncheck "Fill pads" unless you want no drill holes showing in your pads
• under the Layer menu, choose Deselect all
• then choose the Bottom, Pads, and Vias layers in the table of layers on the right
• in the  Page section, give a Height (maybe 2in) and a width (maybe 3in)
• finally, click on the Process Job button at the bottom

i use this to create PDF image files that go into my PDF project files.  if you are unfamiliar with Postscript and PDF stuff, then the first method is a lot simpler.

if i have left anything out, or something doesn't seem to make sense, please ask.  someday, when i have more time, i will put this along with some other eagle stuff on gaussmarkov.net.

all the best, gm

[Papa_lazerous]

Thanks that makes sense, I will have a go at that once I have finished my layout. 

I do however have one more little question though, I am making a TS-808 clone for myself and am using our library as well as the Eagle one for parts.  the only thing I dont know how to do is where I have areas that connect to "Vref" which is my bias I have loads of ares it needs to goto I saw on your site you have labelled each area VR what component in the library is this please. and what component in the library are you using for pots as I have tried "vrpads" and "vrpot" from your library and they dont come out like your schematic.

I know you have got the eagle project file on your site but I dont want to copy I want to learn myself.

I also dont know how put +V and GND onto the opamp I see you have the opamp drawn else where with this connected

Allot to ask I know but appreciation and a favour owed would be returned

[gaussmarkov]

Thanks that makes sense, I will have a go at that once I have finished my layout. 

I do however have one more little question though, I am making a TS-808 clone for myself and am using our library as well as the Eagle one for parts.  the only thing I dont know how to do is where I have areas that connect to "Vref" which is my bias I have loads of ares it needs to goto I saw on your site you have labelled each area VR what component in the library is this please. and what component in the library are you using for pots as I have tried "vrpads" and "vrpot" from your library and they dont come out like your schematic.

you will find VR, +9V, GND, and others in the library gm-supply.lbr.   there are also a +9V(T) and GND(T).  that latter are associated with hookup pads for the layout.  the former are just to provide connections without running wires.  so anything attached to  a +9V hooks up with +9V(T).  we don't usually have pads for vbias, so VR does not have a VR(T) counterpart.  once you find the VR component, hook it up in all the places you need it.

i wonder if you have the latest copy of the library?  the self-installing version of gaussmarkov eagle stuff is out of date.  i have been able to keep the libraries up to date though in this zipped file:  gm-lbr.zip.  download that and copy the library files over the old ones.  in the library gm-pots.lbr you will find the packages "16mm" and "pot";  it's probably the 16mm that you are looking for.

I know you have got the eagle project file on your site but I dont want to copy I want to learn myself.

i completely understand.   good on ya, mate. 

I also dont know how put +V and GND onto the opamp I see you have the opamp drawn else where with this connected

you aren't the first to ask.    another item that i need to post on gaussmarkov.net.  use the INVOKE command.
if you type it in, then you will see which button in the tool bar that corresponds to.  then right-click on one of the op amps
in your IC and a menu will come up containg "P   PWR+- ..." as its last entry.  click on that and you will have the two additional
pins you need for the + and - supply pins on the op amp.  put them anywhere you like, but you have already seen how they
are usually positioned with one of the op amps.

Allot to ask I know but appreciation and a favour owed would be returned

no need.   for me, diystompboxes is not about getting favours in return.  if you have more questions, fire away.

all the best, gm

[Dave_B]

I don't think it gets mentioned enough around here.  Paul did a great job creating libraries with the most used components for stompbox builders.  The only changes I ever make to them are to make the pads a little larger and the drill holes a little smaller.  That makes them easier for me to use. 

I did draw up a VTL5C* opto if anyone needs it.

[gaussmarkov]

thanks, dave.

i always increase the pad size myself.    did you change the libraries or just use DRC Restring?  IIRC, my holes are all 0.7mm in diameter, which i chose because that seemed close to what folks mentioned for practice.  maybe smaller is better, so that one can drill a little away?

I did draw up a VTL5C* opto if anyone needs it.

how about adding it to the gm libraries with your description attached?

[Dave_B]

did you change the libraries or just use DRC Restring? 

I change the libraries.  Once I figure out what DNC Restring is, I may do that.   

maybe smaller is better, so that one can drill a little away?

I end up drilling part of it away.  It makes it easier for me to solder.  The bits I use (from drillbit city) are much sharper than the Hobby Haven bits.   I just need a big enough "hole" for the bit to find it. 

I did draw up a VTL5C* opto if anyone needs it.

how about adding it to the gm libraries with your description attached?

Sure.  Give me a chance to create a "laying down" version of it and I can add it to your stuff.  I have it in a separate "opto" library right now, but it can go in the diode library if that makes more sense.