Welcome to our site!

Electro Tech is an online community (with over 170,000 members) who enjoy talking about and building electronic circuits, projects and gadgets. To participate you need to register. Registration is free. Click here to register now.

  • Welcome to our site! Electro Tech is an online community (with over 170,000 members) who enjoy talking about and building electronic circuits, projects and gadgets. To participate you need to register. Registration is free. Click here to register now.

Help to make PCB with Eagle.

Status
Not open for further replies.

swapan

Member
Friends,
Once I am in need of your help. For my hobby projects I am to design and make PCBs. Recently I have downloaded Eagle software (Freeware version) for making PCB. I have made a PCB (without schematic) of size 4x3 inches. After taking a printout it is noticed that the actual size is 1/8th inch less in length. The width is also less proportionately. The dimension of components and its pinout position is also a little less than actual. Secondly, the pinout pads are so small that after drilling a very thin portion is left. Is it possible to enlarge the pinout pads of the library components?

Swapan
 

Blueteeth

Well-Known Member
Sometimes printers can scale things. I had trouble with my printer 'shrinking' designs, but not as much as 1/8th.

If the length and width are the same scale (as in reduced by the same percentage) then you can decrease the border width in eagle.
The only way I could effectively print out to scale was to scale my design up to counter-act the shrinkage from my printer.

go to 'print setup -> page -> calibrate'

Values greater than 1.000 will increase the size, values < 1.000 will obviously shrink. It is best to create a test design, full size (as large as eagle will allow, 3"x4" if its freeware)
With lines, and pads spaced apart by a KNOWN amount. On the design, mark the length and distance between these lines...then when you print it out, measure their actual values. The amount you must scale is the value its meant to be, divided by the actual value.

Example: your PCB design in eagle had dimensions 4"x3". But your print out measured 3.875 x 2.91. Length (x): 4/3.875 = 1.032 - Width (y) = 3/2.91 = 1.031.

You can of course use the same value for X and Y, but, printers generally are less accurate in a certain axis. So you can scale each axis individually. On mine the length was less accurate (shrunk more) than the width...and it also wasn't very accurate towards the edges of the page..so print your design in the centre of it rather than top left or bottom right.

About pads in eagle library:
I haven't found a 'good' way to increase the size of pads for a ready-made component using a user-language-script (ULP). I'm sure they do exist but the best, and unfortunately, most time consuming method is to create your own package for a certain component. Say you have a DIP16 chip, in an eagle library, and you wish to make its pads larger. Instead of completely remaking the 'device' this is how I do it.

1. In the main eagle window, open the library and find the component of interest (click 'device'), make a note of its package.
2. Now click 'package' and look for the package the component uses.
3. Highlight the whole thing with 'group', then click 'cut', and right click on the package.
4. Make a new package (package -> new) click paste. Then use the change button on the left pane to change the size of the pads. (Diemeter, and shape).
5. Save it.
6. Go to the device again (device), at the bottom right where it has the package, click 'new', give it a random extension like 'mod', and choose the package you just created. Then it'll appear in the bottom right window with a yellow exclaimation mark next to it, indicating you haven't link its pads to pins on the symbol.
7. Click 'connect' then 'copy from' the drop down menu and pick an existing package., then 'ok.

And thats it, you've added a new package to that component. When you choose it in a schematic it'll give two options, the original package, and your own.

It's a really long way of doing it, but you are right, some components like double pin headers, have really small pads, leaving only a tiny ring of copper around them after drilling.

I hope that helps in 'some' way. I've been meaning to make a tutorial for eagle for a while if anyone else is interested in it.

Buriedcode.
 

Boncuk

New Member
Another cause might be the fact that your PCB length is beyond the limitations of Eagle light.

The PCB size limitation is 100X80mm.

A PCB length of 4 inches equals 101.6mm, which is beyond the allowed size. The PCB width of 3 inches (76.2mm) should be OK.

Try to shrink the size a bit and retry printing using scale factor 1.

Boncuk
 

jpanhalt

Well-Known Member
Most Helpful Member
I think the size limitation is built into Eagle lite. One simply cannot place a component outside the limited area.

For changing pad size for a component, I believe you should copy the library component to a new device/package, then modify it. You might be able to simply make the large-pad version as an alternative in the standard library, but I would advise against that. When updating, you probably want the complete new library to be installed. That might cause you to lose the alternative packages (I haven't tried that, so I can't be completely sure).

I suggest you make your own personal library, name it 1<name>. The 1 will make it appear as the first library for convenience. Then add all the things you make or modify to it. When it is update time, all you have to do is copy that personal library to the new version.

If you can tell us what component you want to change and how big you want the pads to be, someone here might do it for you to get you started. Frankly, I have not had a problem with component pads being too small. Maybe your drill is too large?

John
 

mneary

New Member
Change component pad size with "restring". Requires some playing to get the results you want.

Change scale on Eagle's print options dialog box.
 

Boncuk

New Member
I think the size limitation is built into Eagle lite. One simply cannot place a component outside the limited area.
John

Hi John,

your statement is completely correct. I haven't tried yet to draw an oversized dimension layer, but it works on screen.

I made a frame of 140mm length without problems. The component placed within the 100mm allowable length is not to be moved further east.

The destorted print probably means Eagle shrinks the actual board size to the allowed when printing.

Regards

Hans
 

Attachments

  • SIZE.gif
    SIZE.gif
    3.7 KB · Views: 558

jpanhalt

Well-Known Member
Most Helpful Member
Hi Hans,

Thanks for the clarification. I had never tried to do that. I don't use Eagle Lite, either.

BTW, my printer is terrible for accuracy of length. It is not a cheap printer (HP 4101 mfp), and I have just learned to live with it.

John
 

Boncuk

New Member
BTW, my printer is terrible for accuracy of length. It is not a cheap printer (HP 4101 mfp), and I have just learned to live with it.

John

Hi John,

I used the Epson EQL5700 for a board size of 420X280mm (four mounted transparencies) without problems. Even 40pin ICs just dropped into the drill holes without force.

Now I'm using a Fuji-Xerox FX Docuprint 203A which also prints very accurately with equal toner distribution.

If your length error is constant you might average for length and width for the best possible result - or buy a better printer. :)

Regards again

Hans
 

swapan

Member
Thanks Mr. Blueteeth for your kind help. I have tried a lot but could not get the pads modified. Would you please guide me further? Under step 1 you have asked to open library in Eagle main window. By Eagle main window did you mean the window that opens by clicking the Eagle 5.6.0 short cut on the desktop?

Swapan
 

Blueteeth

Well-Known Member
Hey.

Yes, by 'main window' I mean the window that pops up first, when you double click the shortcut.

You can open a Library either by, expanding the 'libraries' on the left pane, then right clicking on a library and choosing 'open', or..
An easier way is just to go to file->open-> library. It should be in the right directory.

The only reason I suggested using the left pane in the 'main window' is because....once you expand 'libraries'...you can expand each library to see what components it has inside.

I have attached a picture...just because pictures are always helpful.
 

Attachments

  • Eagle_help1.jpg
    Eagle_help1.jpg
    164.3 KB · Views: 404

Boncuk

New Member
Thanks Mr. Blueteeth for your kind help. I have tried a lot but could not get the pads modified. Would you please guide me further? Under step 1 you have asked to open library in Eagle main window. By Eagle main window did you mean the window that opens by clicking the Eagle 5.6.0 short cut on the desktop?

Swapan

The window opening is named "control panel" (also main window).

Select "OPEN" --> "LIBRARY" and open the library you decided to change and from there open the package of your choice to either copy or alter it.

If you do not copy you can renumber pads, change shape, diameter and drill. You cannot remove or add pads.

I do not recommend to alter pad sizes of ICs. The pads have an outer diameter of 1.6002mm. Enlarging the pads you can't route a trace of 0.4mm width between pads anymore.

You might want to change the drill size to 0.6mm (from 0.8) for more copper after etching, but then you must use machined IC sockets.

The standard pad sizes in Eagle are made for direct IC insertion with a maximum possible free space between pads.

Boncuk
 

mvs sarma

Well-Known Member
The window opening is named "control panel" (also main window).

Select "OPEN" --> "LIBRARY" and open the library you decided to change and from there open the package of your choice to either copy or alter it.

If you do not copy you can renumber pads, change shape, diameter and drill. You cannot remove or add pads.

I do not recommend to alter pad sizes of ICs. The pads have an outer diameter of 1.6002mm. Enlarging the pads you can't route a trace of 0.4mm width between pads anymore.

You might want to change the drill size to 0.6mm (from 0.8) for more copper after etching, but then you must use machined IC sockets.

The standard pad sizes in Eagle are made for direct IC insertion with a maximum possible free space between pads.

Boncuk
for IC, it appears OK
but for normal components and Vias , the drill hole size appars too big leaving a thin copper surrounding it. that small ring would likely be peeled off during drilling.
3v0 suggestion is OK if implemented before tracks are routed, otherwise, the tracks would be just fouling with pads, perhaps. Not clear whether DRC would take care this , after adjustment as suggested by 3v0
 
Last edited:

3v0

Coop Build Coordinator
Forum Supporter
I do not run DRC till after all my tracks are routed.

You can freely change RESTRING and Clearance at that point.

If restring causes a trace to be too near a pad move the trace.

DRC allows you to accept errors, For eaxmple the space between pads on a cap may become too small with a large spacing and restring value. Or the space between pins on a SMD part.

If needed I will show some PCB.

3v0
 

DirtyLude

Well-Known Member
Somebody posted an Eagle script a while ago that fills drill holes and leaves a smaller hole just to start the drill bit. It sounds like what's trying to be done here. I don't remember the script, though, and I'm too lazy to look.
 

Odin

Member
Somebody posted an Eagle script a while ago that fills drill holes and leaves a smaller hole just to start the drill bit. It sounds like what's trying to be done here. I don't remember the script, though, and I'm too lazy to look.

drill-aid.ulp is the name. It draws additional pads in a new layer, with the inner diameter you choose.
 

prabhueng

New Member
Hi all,

If I am not wrong, it is not needed to create a separate library with the selected components.
It will create some headaches like we need to save the library and if we install the later version of EAGLE means we need to update the library.

It is very simple to use DRC in the EAGLE. If u open the DRC window means it has many tabs.
Correctly enter all the values. The mains tabs for the homemade PCB's is the restring and the clearance tabs. Choose the appropriate values for them.

I made the several circuits in the home.

IF u want i will send the drc file of me.
 

jpanhalt

Well-Known Member
Most Helpful Member
The biggest problem with using the restring tab in DRC is that it seems to affects all pads. That may not be what a user wants to do.

In DRC is there a way to change the pads of just one component?

John
 

3v0

Coop Build Coordinator
Forum Supporter
The biggest problem with using the restring tab in DRC is that it seems to affects all pads. That may not be what a user wants to do.

In DRC is there a way to change the pads of just one component?

John

Not that I have seen. I think it is time to look at some artwork and the clearance and restring values used.

3v0
 
Status
Not open for further replies.

Latest threads

Top