prototype pcb design

JonSea, great, I already got some ideas from Ian Rogers but I had some still unposed questions about replication which I do not understand too well yet in Eagle.

Your post seems to answer those; creating packages and symbols are not a problem anymore, so that will work. Copy and paste will be part of the learning curve.
Tomorrow I will give it a go with your instructions and keep you posted here.

As far as the limitations for the low-cost board at the fab is concerned I need to verify.

Have a good day, thks,
Erik

To "copy & paste" in Eagle, you "cut" an item or a group using the scissors symbol. Despite the name, "cutting" something doesn't remove it.

"Copying" something in Eagle as done with the symbol that looks like stick figures, copies the selected item or group once. To make a second copy, you must select the item or group again....so if you're copying a group, first you have to select the group, then copy the group. It's a bunch of extra steps in this case.

Eagle's concept of a group is a little different too. You can't make items part of a group permanently that keeps them all together - a group is a momentary collection for the following operation only.

JonSea said:

Eagle's a group is a momentary collection for the following operation only.

Click to expand...

Just one small point: the selection (group) remains valid until you make another selection. So you can copy, move, delete etc a group as many times as you like.

Select the group. Click on the function you wish to perform on the group from the menu at the left. Right click on any object in the group and the pull down menu will offer the function you selected from the menu at the left.

To deselect a group just select another group on a blank part of your drawing.

You can select a group in two ways:

(1) Click and hold. Then drag a rectangle over the items you wish to group and release the mouse button.

(2) Alternatively, you can use random polygon select, which is the most flexible: Click and release near to your intended group of objects. Move to a new point and click and release again: a line will joint the first click coordinate to the second click coordinate. Continue clicking and releasing until you have enclosed all the objects required. Then move to the first click point and double click. The polygon that you have just drawn will be shaded and all the objects within the polygon will be grouped. While you are clicking coordinates you can cancel a point by pressing escape.

You can not only copy groups on to the current open sheet, but you can also copy groups between sheets.

With some of the ECAD packages selection can be a bit twitchy, but in EAGLE it works a treat.

spec

This is literally about 5 minutes of effort. sorry for the picture quality...it's a screen shot of the computer screen from my phone.

JonSea said:

(...) This would consist of 3 pads at 0.1" spacing of the appropriate diameter, with a trace connecting them. (...)

If you want to make continous "bus" strips at the top and bottom, duplicate the rows 2 more times. Then use the air wire tool to connect all the 3 pad groups in the row together and route a trace between them all.

Click to expand...

Hi JonSea, I have no idea how to connect the pads with a trace: how do I do that?

"Duplicate the rows 2 more times", and "airwire tool": can you explain more please? And "airwire" I cannot find.. ?

Thks,
Erik

...something like this? I used the wire tool linked to layer 1.top in package to connect the pads: correct?

My advice as follow:
1 understand the schmatic, what is this pcb use for
2 design it with proper line and via diameter
3 saving the cost of the board by design
4 design for easily manufacturing

There's actually an easier way to do this. I'm going to post pictures of each step just to cover the bases. For all of the following, I suggest setting the grid to 0.1" or whatever you want the spacing to be - the last picture below shows how to do this.

1. Start by putting 3 pads (vias) on the board. You can select the shape you want, the hole diameter, and even adjust the angular ring size. (See corresponding picture below.)

2. Select the "wire" tool, and the top layer (or bottom - it doesn't matter in this case) and connect the first two pads together by drawing from the center of one to the next.

2A. A dialog box will pop up asking if you want to connect the signals together and what name it should be. Click ok to accept the default option.

3. Group the 3 pads and traces by selecting the "group tool" and dragging a box around them.

4. Click the "cut" tool on the left.

5. Position the cursor in the center of the first pad. Right click and select "cut group" from the bottom of the pop up box.

6. Click the "paste" tool on the left and the group of pads will appear.

7. Position it in line with the first group. Repeat to create as long a row as you like.

8. Group, cut and paste the entire row as many times as you'd like.

9. Using the wire tool, connect the groups along the edges to make a bus along each side if you'd like.

10. The completed bus.

11. Click the "wire tool" and select "Layer 20 - Dimension" at the top. Draw the board outline around the pads.

12. You may want to add mounting holes at the corners. I use a 0.125984" / 3.2mm hole which works well for 4-40 or 3mm standoffs.


I think this should cover all the steps. You can add embellishments to make it your own: rounded corners, maybe a column of 2 connected pads at the end for a header connector, perhaps silk screen labels to identify the rows and columns (if you're going to label the top side, you make want the traces on the bottom side)....

Whoaw, great, thanks for this explanation.
Just a few questions:
1. Now to come back to your initial proposal, which is to use the "package" tool first: why not use that route?
2. I used in my post #26 the "package" route and connected the pads with the wire tool using layer "1. top": is that correct (as long as the pads are in layer "1. top" too)?
3. Your post #28 uses the .brd to design the copper tracks: what if I do not need copperplating in the holes, (how) can this be done with the "via's"?
4. Your post #20 does not show whether layer "1. top" or layer "16. bottom" should be used: is that not required?

Thks
Erik

..and here another one: post #28 uses vias for the holes, however components need to go through the holes so by definition a pad with a drilled hole should be used (vias are not meant for component placement)? So, this is back to the "package" option (post #20)?

Why not a package? In this case, it's just a extra step that doesn't buy you much. Also, Eagle doesn't really like traces in packages (pcb footprints) so in some cases they don't behave as you expect (but the Gerber files will be fine).

I think in #26 you didn't run the trace from hole to hole, but merely overlapped it with the pads. This should work ok, but could lead to some issues when you have the boards made (a trace between holes WILL connect them, a trace overlapping pads may not depending on tolerances in the board layout process).

Eagle calls plated-through holes vias. A tiny hole is a via. A larger hole is a component pad - there is no difference.

Does your board fab house actually make single layer boards without plated holes? I don't think mine does. If they do, they probably don't plate the holes anyway, so the use of a "via" won't matter. I'm not sure Eagle even has a mounting pad that's not plated. I'll look a bit in a little while.

Interesting, JonSea.
So, if the Gerber files show that the connection is ok, does that mean the actual pcb will be fine too? Regardless of the fab house? Or did I read your first paragraph in post #31 wrong?
I do not know -yet- if the fab house I use (Elecrow) makes single sided boards without plating holes.
But if they don't what would be the drawback (of having plated holes)?
If the overlap between the pads and the trace in my proposal of post #26 is not sufficient would it help to enlarge the trace?
I feel (subjective opinion) that the advantage of using the package is that Eagle allows quite some finetuning in the package.

If I use vias can I make the via hole diameter as large as I want (for example 0.035")? And can I make the wire connection between the vias as large as the via width itself (up to 0.075" or so)?

Elecrow does make single layer boards (I suspect the holes are plated), but there's no cost savings to do so. A plated hole is easier to solder but the downside is it can be harder to unsolder a lead. The trace between the pads can be as large as you like but a 12 mil or 16 mil trace will likely handle anything you do on a prototype board.

There's no reason not to do it as a package if you want to.

Ok, I will try both methods and if ok with you post the results for your critical review. Will be a couple of days.
Thanks for your help!
Erik

Just to verify to myself....

This is the Gerber top copper layer. In the bottom 4 pads, the trace was drawn from pad to pad to pad. Eagle considers all these pads connected together.

For the top for pads, the trace was dran from the first pad to the last and just overlays the center pair of pads. Eagle does not consider the center pads to be connected to the pads and in fact, a design rule check would should errors for overlaps.

All the Gerber file knows is where the copper is and has not idea of your intentions - the two sets of pads are exactly the same as far as the Gerber file (and therefore circuit board) are concerned.

Whoaw, great! Thank you for the check, very usefull. I am currently busy with the pcb's (post #34).

Seattle must be past midnight??

Nearly 1 am, and I'm going to bed

Here are the 2 .brd files, the first is made with pads in packages, the v4 with vias direct in the .brd.

1368 holes each.

I took a grid of each board to show here. It will be easier to understand.

In version one, you've overlapped the gap between pads with a trace. This is a unique approach to say the least; one I don't recommend.

Going from Gerber files to a board is a photographic process (it may be digital now, but the same concepts apply). The copper for the pads is made by using an aperture to expose the pad area. There is some tolerance in this process both in terms of pad size and of pad position relative to the drilled hole. The traces are made by a difference process. The trouble with this method is that the traces don't connect the pads as is the usual case. There's no guarantee that the traces connect the pads if the tolerances are off. It probably will work ok, but why bastardize the technology?



For version 4, it took me a while to even figure out what I was looking at.



Turning off different layers made it more clear. Square pads and a big thick trace connecting them.





This will work fine for board production. But to be honest, from a use point of view, I don't think this is optimal. The thick trace isn't needed for anything you're likely to build on a proto-board, and the large pads and traces end up being kind of close together, increasing the chance of solder shorts between pads.

If you're trying to duplicate the proto-board you showed originally exactly, this won't quite do it. The area in between the pads will be covered with solder mask - it won't be a 1x3 area of blank copper. More on this shortly.

Here's what the Gerber files for version 4 look like (for a small section).

This is the copper layer.



This is the soldermask layer. It's inverted, so the colors indicate where the soldermask is NOT - i.e., the areas that can be soldered.



Showing both together shows the squares of the pads separated by the soldermask.



This isn't a problem at all, but I don't think it's what you're expecting.