Hello there

I am working on a project which involves the development of a pressure sensor matrix capable of pressure mapping the force applied on a patient by a medical instrument.
The active measuring area consists of a matrix of 28 interdigitated electrodes on a PCB.
I am trying to design this, but I am having some trouble with the autorouting.
When i press the function it stays in 0% and doesnt seem to even start the process.
I played around a little with the design rules, but I am pretty new to this whole world and I am sure my problem is somewhere there, I just cannot seem to find it

Unfortunately it does not let me attach the EAGLE board file here, but if anyone has any idea what it could be and has the time to help me out, please contact me and I will send you the file somewhere else, so you can see my design for yourself.

I hope I am making sense here, and I really hope one of you out there with more experience can help me out!

Thanks a lot for your time

 

Does ERC report any problems?
Is it allowed double-sided routing?
After that it may be your custom library part and/or design rules.

 

I have a ton of errors (attached below) but I dont know how to fix them. There is no other way i could net the pins..but somehow there seems to be no connection between them.
Autorouting on both sides is allowed.
Is it possible for you to check my schematic file please? I could really need some guidance. I have been stuck on this for days now.

Thanks a lot for yourreply and your help

 

I tried to load your schematic in Eagle 5.2 but it won't load. What version of Eagle are you using?

A few more things:
In error1.png, it says it can't find the board. The schematic and board have to have the same filenames and both have to be loaded while you edit either so that forward/backward annotation can be done (to keep the schematic and board consistent). That annotation process is what builds the netlist that the autorouter uses to know what to hook to what.

The warnings are from the schematic and indicate that you have missed connections. Those close but unconnected nets may not be added to the netlist. Go back and fix all of the 'unconnected' and 'overlapping' warnings.

When you look at the airwires on the board, what do you see? These are on the Unrouted layer 19 (on mine). To show them, turn on the airwire layer and click the 'Ratsnest' icon near the bottom of the side menu. It should show the entire circuit in lines that run point to point. The autorouter (or routing manually for that matter) uses the point to point netlist to know what to connect. No airwires, no autorouting. Even when routing manually, you have to grab an airwire and route it to completion to make the DRC/ERC happy.

Be sure that your zigzag contacts are on a signal layer. Use Identify to make sure that they are connected to the net you expect them to be. Since you have missed connections in the schematic, the zigzag components may be assigned to another net with no connection.

Make sure your connections on the schematic are on the 'Nets' layer. Remember that even though the visible lines in the schematic may overlap, you have to make an end to end connection between the wire and the actual connection point on the component symbol. You can view those points by turning on the 'Pins' layer in the schematic. The wires on the nets layer have to connect to the component inside the little green circle. Keep the schematic on grid and have 'Snap to Grid' turned on always.

Once you get all of that fixed, consider manually routing the board. I've found that except for very orthogonal stuff, the autorouter is more trouble than its worth, even on larger boards. If you have your netlist right, clicking on an airwire will jump a trace to the connection point and follow your routing to its endpoint. Simple.

When its done, I recommend that you turn off all visible layers except the airwires to look for any missing segments. These are usually due to a track not hitting the center of the pad or other off-grid stuff but I resolve these so that the ERC can find any missing stuff.

Good luck.

 

On your schematic, eagle will not connect wires to what look like the pins on your electrodes. How did you create these? As a library part? If so, include the part.

 

I have a ton of errors (attached below) but I dont know how to fix them. There is no other way i could net the pins..but somehow there seems to be no connection between them.

Did you have the grid set to some sane value? Turn off all layers except "unrouted" and you should be able to see all of your almost connected errors.

Autorouting on both sides is allowed.

I never use autorouting. The routes are invariably non-optimal and messy looking. Your board is small enough that manual routing shouldn't be difficult.

 

1) Use net, not wire to connect things in your schematic.
2) Failing that, you can wiggle things to see if they are connected.
3) Fix the "not connected" and "overlaps" and then come back with a reasonable number of errors for us to look at.

Regards, John

EDIT: To re-emphasize some of the earlier posts, ERC is very important. There may be errors, but they must be intentional (such as unconnected pins). Never try to route until you are satisfied with the ERC. Now for DRC, there are probably more exceptions, depending on your settings.

 

Hey, thank you all for your quick answers!
I seem to think thatthe problem is with the custom library part, as I said im very new to EAGLE and I have been teaching myself throughout tutorials only.
My customed component should be just copper tracks consisting of an upper and a lower structure that dont have any contact between them, a pin which is connected to the upper body is supposed to take the signal from it, and a pin on the lower body takes the signal from the lower one. The nets should work on the following well: all the upper pins from the upper structure of the electrodes of the first row should be connected, as well as the ones with the second row, third row and so on. They represent the value for each row (7 of them in total).
The lower pins on the electrodes should be connected in columns, like this: first electrode (from right to left) on the first row, connected to the first electrode on the second row, as well as the first electrode on the third row, and so on.The same is done to all the columns (5 of them) and this nets will represent the values of the columns. My goal is to create a matrix array which displays the force distribution.
When creating my component, I used the function Keepout to cover my electrode (except the pads) to avoid tracks running through them, since my design, and I forgot to specify this before, will be fabricated on a sheet of flexible, double sided polyimid copper clad laminate. This means I am very restricted to the size and layers.
I changed my working grid both in the schematic and the board to mm (I am European and working with inches makes me really confused), could this be a problem?
The custom library is attached below.
Thank you again for your help, this really helps me getting forward!

 

Changing the grid can cause a problem getting things to connect. That was a bigger problem with earlier versions. Current versions snap to the center of pads, in theory. Some users say "never" change the grid. I use the grid settings as a tool on occasion when making a package or routing, but always begin and end with the same settings. Changing the grid is (much) harder to justify when working on symbols and schematics. I would recommend not messing with the grid settings until you are more comfortable with Eagle.

It is tempting to make symbols and packages look just like the actual device. That can lead to problems and unnecessary complexity. On some occasions, I have used a simple rectangle with a identification in it. All you really need to have correct are the electrical connections and pad positions. Here is a component from my heating system as an example:


Have yo made progress on the ERC?

John

 

Working on fixing the ERC i have come across some doubts, that I hopeone of you couldhelp me out with.
I followed your advice to change the components to simple resistors, to make sure if my custom part was the problem. I still get the "net overlaps pin"error on the ERC, could someone explain to me what this means? is there a certain way to connect a net to a pin?
The "no pins connected to Net" erros still appears as well, and this just gets me even more confused how do i make sure the nets are being placed on a working area?
Thanks again for the help!

 

What version of Eagle are you using? One cause of the overlap problem is when you change the grid size. Grab the net and wiggle it. If there is overlap or no connection, that should be obvious. Also in the layers, show pins (layer 93). That will help you see what's going on. The connection is at the center of the open circle, not past it.

EDIT: There are some ULP's that may help. This one looks attractive: snap-on-grid-sch.ulp
That should at least get your symbols on whatever grid you are using, then don't change the grid. If your symbols are made with imperial units, then I recommend that you use 0.1" grid.

John

 

Follow-up
This is from your first schematic:


I simply "wiggled" the part, and you can see that no nets are connected to it. Please post you most current schematic, if you still have problems with it.

John

 

You can use a data compression program, like 7-Zip for Windows, to create a .ZIP format file for upload here. .ZIP files can be much larger than other types of files.
You can download 7-zip here:
http://www.7-zip.org/download.html
One of the first 2 listed should work with most Windows versions.

 

The device which you created has the pins misaligned. The pins on the symbol need to have their connection points on the junction of the 0.1" grid, or you will have a difficult time connecting to it in the schematic. Ideally, the + sign in the lower left corner should also fall on a grid junction, so it is easy to align on the schematic.

When on the schematic, you almost never want to change from a grid of 0.1 inch; as you will likely wind up with problems. If you DO change it for some special reason, change it back ASAP, or you will spend a lot of time un-doing and re-aligning things.

Try to avoid making wire corners other than 90 degrees in the schematic, keep the bends and wire crossings few. Lots of corners and angles make the schematic much more difficult to read.

It is a good idea to start a schematic drawing by dropping a frame in with it's + at coordinates 0,0. I suggest starting with FRAME_A_L, which is an "A" size drawing (8-1/2" x 11") in Landscape format. If you don't start with a frame at 0,0 it will be difficult to tell where you are, and your printouts will likely take several pages where one would otherwise do. You can always change to a larger frame size if needed.

 

Hello again

First of all I would like to thank you for your advice and guidance, you are all incredibly helpful!
After following your advice, I have finally managed to create a schematic that passed the ERC clear!!!
It was a grid problem mostly, I had to play around with that a little, allign my component and pins and I worked with the default grid, which functions way way better!
I have come across new problems unfortunately, now in the board file, at the moment of trying to autoroute my tracks.
At some specific percentage (80.4%) it simply stops doings its job and doesnt seem to process anything at all.
Because of the little space I have available for my design, routing manually wouldnt be an option.
Anybody have an idea on how I could overcome this?
I am attaching the files both schematic and board below.
Thanks alot for your help once again!

 

I don't understand why you have concluded that manual routing is not an option? How many boards previous to this one have you routed manually?

Many users, including myself, never use the autorouter for actual routing. At most, I will give it a try to checkout various component placements, then I rip up everything and route manually.

John