Need some help with Eagle and pads vs vias et al

[tagaide]

Hi Everyone.
I am trying to create a simple board design for a keyboard matrix using metal domes as switches.
The schema is easy enough, i first created a custom library which was essentially wire for the outter ring (contact) and a pad for the inner contact.
see image



I then found someone elses library for omron's dome keys which is made of smd for the outer contact and a pad for the inner contact

see image



in both cases,
the outter contact or ring is attached to the rows and the inner one on the (2nd layer) back of the board.

Now. come the questions.

1) which of these libraries is correct the smd + pad one? considering i want to make a double sided board.
2) how do i draw the board. i have drawn the top layer by connecting all outter rings per row and the bottom layer by connecting all the inner circles by column using the wire tool,
3) am i correct in saying that i need vias and i need to make them in the board design tool and not in the library itself?
4) or do i just need to draw a hole.

the biggest issue i am not sure about how to solve is that regardless of smd or wire, how do i make sure both sides are correct and how do i add the via.

You can probably sense i am quite a noob. any help is appreciated. if you need more info or pictures let me know.
thanks.

 

[tagaide]

Right, i will be happy to rephrase this if that makes more sense. its a steep learning curve for me.

 

[jpanhalt]

Hi Everyone.
I am trying to create a simple board design for a keyboard matrix using metal domes as switches.
The schema is easy enough, i first created a custom library which was essentially wire for the outter ring (contact) and a pad for the inner contact.

That is a good start. A lot of new users won't even try to make a custom library.

Now. come the questions.

1) which of these libraries is correct the smd + pad one? considering i want to make a double sided board.

I don't know that there is a correct or incorrect one. But your device might be a little ambiguous in that the outer ring does not have a layer associated with it. How will the manufacturer know which layer to put it on? Using the red (top) layer for the ring will avoid that potential confusion. You certainly wouldn't want that entire outer ting made into a via. So, if I had to pick only one design, I would pick the "SMD" version.

2) how do i draw the board. i have drawn the top layer by connecting all outter rings per row and the bottom layer by connecting all the inner circles by column using the wire tool,

The wire tool will work, but I would recommend using the "net" tool. It helps avoid overlaps that are not electrically connected.

3) am i correct in saying that i need vias and i need to make them in the board design tool and not in the library itself?

I don't see how the inner pad can be connected to the bottom layer without a via.

4) or do i just need to draw a hole.

the biggest issue i am not sure about how to solve is that regardless of smd or wire, how do i make sure both sides are correct and how do i add the via.

That is where using the proper layer and tool coupled to the schematic helps. Be sure to run DRC (checks the board) and ERC (checks the schematic). Eagle will prevent you from drawing a "connection" that is really not a connection. It also helps with the mirroring of one layer. If you get an error, such as a layer violation (I am not sure exactly what it is called, but that is what it means), please upload your board file so we can help you work with it. The pad/via tool adds the via.

John

 

[tagaide]

thanks jpanhalt.

Would it be ok if i upload my (new smd style) library and schema + board for you to give pointers on.
I think i can handle the vias part when i see an example of one. because there is no 'real' smd (well, the metal dome is )its hard for me to grasp the concept of connecting it all up in a board design.
Thanks so much already.

 

[jpanhalt]

Just upload your board and schematic here. Those are allowed file types. No need to include your library. It comes with the schematic file.

John

 

[tagaide]

i am getting there. currently while more or less replicating the smd style library i am stuck unable to wire up my columns.
anyway i will post the files, i am sorry this is dragging on. I am very much commites but it is the usual getting to know the toolbox issue.

thanks for your patience.
files will be posted in 10

 

[tagaide]

attached the files. not that at least using the wire and pads i was able to get a proper connection for both rows and columns.
Now, it just does not seem to work, the essence of the question is still how to draw vias given this is a 2 layer board based on the library.
thanks a million again!View attachment sample.schView attachment sample.brd

 

[tagaide]

sorry m i tried upping the librarie files which failes unfortunately.
i can make a screenshot of the package or symbol if it helps?

 

[jpanhalt]

1) When you need to upload something that is not an allowed file type, just zip it, then upload. That may be the problem with the upload, but I am not sure.

2) The schematic, board, and snap switch device seem to have problems.

a) First, run ERC (electrical rules check). You will see a large number of errors, including overlaps and non-connections. One way to test for non-connections is to wiggle the symbol with the move tool. If the wire doesn't move with it, it is not connected.

b) One cause of non-connects is when you change grid. If the device/symbol are placed using different grids, and you are wiring with maybe a third grid, you will inevitably get disconnects. Up at the top of the drawing area you will see a button for ULP (user language programs). There are some very useful routines there, and others can be downloaded from Cadsoft. I tried "snap-on-grid-sch.ulp" and it helped a little. There is a major grid and a minor grid (alt key). There have been disagreements about using alternate grids on this forum. I do, but I am also very careful. Until you are comfortable with Eagle, I suggest you stick to the default grid and an alternate that is a simple fraction of it, such as 1/2, 1/4. or 1/10, etc. A problem that comes up is when a component is drawn on a metric scale, say 2 or 2.5 mm spacings, and something else is drawn with 0.1" spacing.

c) Finally, the component seems to lack a suitable "pin" on the outer ring, which explains some of the non-connects and overlaps. If you click on "show" pins in the layers dialog (button with colored sheets) you can seen a bunch of gibberish by the device. That device needs to be redone. Make the symbol, package, then combine them into a device.

I have attached a saved version of the schematic and that I manipulated. They may be the same since Eagle links the two, but I can't check that without posting then downloading them again. Just checked, they are the same. You only need to open one.

John

 

[tagaide]

Thanks, it complains about invalid file and will not open. i am running a slightly older version of eagle 5.11.0 for Mac OS X.
The pins are the biggest problem, because i am essentially placing many smd's to make the outter connection.

I have attached two files,
works not mine.zip this is the working example, select the closed dome device.
fails mine.zip this is the one i made and used, there is only one device.


i have ran through the repeatedly , did found i had to use @ sign to group them but with no effect.

its a bit awkward, i wanted to know how to desing the baord with vias but now i am stuck getting a library done.
View attachment failsMine.lbr.zipView attachment worksNotMine.lbr.zip

thanks for your help.

 

[jpanhalt]

I used ver. 6.2.0. Once you open and save with that, it is not backward compatible. I will use an older 5.xx version from here on.

Don't have any time this morning to work on it. It will be away about 6 hours before I can spend spend time on it. Where did you find the commercial library for the device? Was it downloaded from Cadsoft?

John

 

[tagaide]

I found the library here.

thanks again John.

 

[jpanhalt]

I found the library (link>dome-key.lbr>dome_bd3_open.sym) you used and adapted it to what I think you are trying to do. I have not prettied it up with names, values, and such. All nets need to be connected to a device or they don't show on the board. I used 1X1 pinhed for those connections. They are easily changed. I am assuming you will be using some sorte of nx1 header/receptacle for connecting to the key-pad.

The library device that was imported does not pass DRC or ERC. I did not try to fix that. If I were doing it, I would design it differently. I forget how many pads were used to make the outer ring. In theory, that might allow one to attach almost anywhere, but I can't see any real advantage to doing that versus a single attachment point. Another question is why the ring is made open. I did add vias to the central contact, like I think you wanted.

Anyway, here is a zipped file to start with. It was made wit 5.11 and should open with what you have.

John

View attachment Dome-Key.zip

Oops, somehow board and schematic link got broken. Just load them together before doing anything to either and it should be re-established.

 

[tagaide]

Thanks a million, this is great.

 

[tagaide]

hi John answer the question 'why did they leave it open'. the open connector is for single layer boards, i was working on the double layer , the closed outter contact one.
I am going to step through every value and name know to make my version of the lib work. your work on the vias make things more clear now. One thing i would like to ask is. The actual connecters (outter rings) did you just connect to them or did you draw on them with the line tool?

I have received more information than i could have wished for already. thank you so much!

 

[jpanhalt]

Yep, the reason for the open end was obviously for a single sided board. I kind of liked the packages with the squiggly lines for the contacts.

As for what I did to the library, I noticed that its author used lots of pads to create the outer ring and then carried them over to the schematic. It can be done that way with grouping, as you suggest, but it is a mess (IMHO).

I simply added one pad to the schematic after deleting the others in the library edit window, and then when making the device, picked one of the multiple pads that was in the location I guessed you wanted it to be in. I haven't actually made this type of device before, but if I were to begin fresh, I would probably make a custom pad or use a copper pour to fill in the rest of the ring. I can see having multiple contacts to the ring, say four at a 90° spacing. Then the top layer would just be direct connects.

I would suggest updating Eagle to at least version 5.11. 6.0 is enough different, but has more capability, that you may decide to wait for that. Eventually, going to 6.xx will be unavoidable because of the backward compatibility issue. That is why I keep 3 versions installed on my PC. Once you install 6.xx, you have to be careful about opening work done with older versions and modifying and/or saving it, as you saw happen in this thread.

John

Hey, I just noticed that ETO automatically translates acronyms such as IMHO. I wonder that the whole list includes? MVBFF -- I guess the list is not complete.

 

[tagaide]

Here is the spec sheet i am using for the contact,
my intention is to use the 5mm variant highlighted green.
What is the best way to draw the outter ring and hook it up to a symbol.

The sizes are quite critical as i need to place many domes on a small board. I want each row and column to connect to a pad i can solder to my controller using plain wire. the board itself will be double layer one.

 

[tagaide]

post by jpanhalt.
I gave it some thought yesterday. The hardest problem may be the off center via, assuming we are both on 6.xx. But even that is probably easy.

1) How many connections do you need to the outer ring? I suggest either 1 or 4 at 90°. If one, then the little bar that is shown is it?

2) As for the via, how small a hole can your board house through plate?

 

[tagaide]

note the outer ring should be closed and the center contact is expected to be a via.
1) i think more contacts give more flexibility but i think 2 are needed at minumum to daisy chain the connections? might be wrong here.
2) The intention is to mill the board on a cnc machine, i think 0.8 milimeters is possible for the via.

this is for my initial prototype, i found a tutorial on the internet from a guy who made vias by sticking copper wire in the holes and placing the board in a press. i will try and do the same.the maximum amount of buttons , domes i will be placing is 10 columns * 8 rows.
it will be less after initial protoype.
The rows and columns of the board will be connected to a teensy 3.0 using plain wire.

 

[jpanhalt]

OK, I will put 4 pads in the outer ring and only the via for contact in the inner. The @ symbol will be used so they will not each need to be connected. Note, the inner circle is only 2.03 mm diameter. I just noticed that the spec sheet does say the off center hole should be 0.41 mm (0.016", #78 drill). You might want to run that past the person who is making the board for you.

As for using the small wire method for making a via, that may change the contact properties. That is, make a bump. If carefully soldered, you can keep the top a smooth, flat dome.

John