Unlike most of Willie’s boards, the one I am making has to be round, and it has several holes for both mounting, and to transfer battery power, as the board has to fit inside that space at the top of this prototype battery holder:
Just draw a circle in your “dimension layer”, then either send a separate dimension gerber to your fab; or have the cad output combine it into one of the silkscreen layers, and tell your fab to cut to that.
I will have to play with it a little, but I think I understand the advice you are giving me about the work-around with the dimension layer and then working with the board house to make it work, but I have to admit I am nervous about something going wrong.
So basically Eagle does not have built-in or pre-defined “round” or circular board as an option?
Well; the pre-defined board you see is just a bunch of lines drawn in the dimension layer, nothing more. This isn’t really a workaround, more the proper way of doing things!
Basically, your fab just needs to know where to cut. Some fabs like to get a specific gerber with the edge that needs to be cut, some are happy to do it to a line in the silkscreen, it all depends on the fab. The same applies to having a rectangular board made!
perhaps you don’t understand. The board outline is defined by the dimension layer. There’s no magic involved. Try it:
turn off all layers but “dimension” (not necessary, though)
delete the outline that is there
use the circle tool, make sure the dimension layer is selected
draw your new outline
turn the other layers back on and start placing/routing/…
Now, you will find that eagle will respect the circle as the outline of the board. polygons will get clipped to it. drc will complain about parts and traces too close to the edge and so on.
Until just now that I read your replies, no, I did not get it - thanks much for taking the time to explain it again. I did not realize that it was that simple, as making the changes in the dimension layer. I also did not realize that I could define vias with a hole that big - definitely I still have LOTS to learn.
Well, I am going back to work on my design. Hopefully it will go easier from now on.
Well, it’s not quite as easy to make a round PCB if you wanted a ground plane. For that, when drawing the ground plane polygon I find the four compass points of the circle and then use the arc linetype to create a circle from four arcs. It’s very finicky because the arc linetype will want to invert right at the 90 degree mark sometimes. Often you can get around this by rotating that line segment later.
Or write a ULP that draws a polygon circle from lots of small line segments.
OK, guys, an update. Just like you guys said, creating the round board was piece of cake in layer 20. Now, I can easily create the VIAS with the outer diameter and drill hole that I need, but I have not been able to figure out how to manually “connect” the input/output signals to those VIAS that I have defined. I think it is something really simple, but I just can’t figure it out. Maybe I should not be defining the vias before hand?
If you create the VIA before hand, it’s assigned a signal name of it’s own. In order to connect it to a signal trace that you’ve got in the schematic you need to name it the same as the signal you want it associated with.
If you want to run your power line through a via that you already have placed on the board, use the EDIT->NAME tool and select the via. Change the name of the via to the same name as the name of your power signal (VDD, VCC, V+…) Once you change the name, the via is associated with that power line and you’ll be able to connect it using the regular route tool.
Usually people use the route tool, then change the layer where they want the via to appear. If you switch layers while laying down a trace, a via will automatically be dropped. Alternatively if you place a VIA directly on a trace you’ve already laid down. It will automatically be named the same as the signal it’s on top of.
OK guys, here is my latest iteration of this board.
I had to define a new pad with a large hole so that I would have an exposed copper area, as using a via for a hole would have solder mask around the via and it would not be conductive.
Now, I am doing here some things I am not sure if they are right. Besides the 3 conductive pads for the 3 rods, I also need to plain holes - I don’t care if they are conductive or not as they have no electical connection to the board. I just did 2 circles on layer 20 (dimension layer) which are the top most and right most “holes”, but I am not sure if that will make the manufacturing board drill holes in there or not. Ideas?
Also, I am getting a few errors that I can live with (some dimension errors about being close to the edge and so forth), but I am getting some “drill size” errors on my vias, but I don’t know what is wrong. I am also getting some “stop mask” errors, which I guess are about clearance issues?
I feel that I am now very close, but need a little bit of help to get this one ready for first pass on a manufacturing house.
min drill size for a via is controlled by a DRC tab. I believe it’s set to 24 mil. As long as the actual size is above the GP minimum, it will be ok. I think the error arises due to a metric ↔ imperial units switch that makes the default via size slightly less than 24 mil.
Philba:
min drill size for a via is controlled by a DRC tab. I believe it’s set to 24 mil. As long as the actual size is above the GP minimum, it will be ok. I think the error arises due to a metric ↔ imperial units switch that makes the default via size slightly less than 24 mil.
OK, I will check on that tonight - thanks.
leon_heller:
Why is the routing so untidy?
Leon
Philba:
there appears to be a lot of off-grid stuff. I suspect the OP hasn’t master the fine art of dealing with Eagle’s quirks in this regard.
The OP (me) has never done a board before. It is my very first board ever, all surface mount, the outer size is fixed for this application, and so are the locations of those holes for the rods, so I am not expecting to do everything perfect - not by a long shot. In fact I am expecting to make lots of newbe mistakes, which is why I am posting here to get pointers/suggestions/ideas/etc..
However, I do need a little bit more specific feedback. What do I change to make the routing more tidy? When is it tidy enough?
Everything is on-grid, but I had to change default grid (it was too coarse) in order to get enough clearance between wires for several of the surface mount parts. Suggestions?
I still need to know how to make those two holes, the ones without an electrical connection. I am really looking to learn, so all feedback is much appretiated
leon_heller:
Tracks should be straight, not curved, and bends should be at right angles (mitred) or 45 degrees. You shouldn’t have odd bits of track at a junction.
Leon
Ahh - got it now. I understand what you guys meant. Let me work on it some more - that makes sense.
I’ll give you an example - IC1, pin 2 to R5. I would leave the top via (near IC1), ripup the rest of the trace to R5. Then I would route FROM R5 to the left, create the via (by changing to the bottom layer) and route up to the other via. You got a weird little “dingle” there.
I would select an alternate grid of 1/4 the standard grid size (probably .0125) and use that to keep your traces much tidier. hold the alt key down when routing to see the effect. Also, when you route to an off grid pad (for example all IC1’s pads), you will have trouble getting the trace to line up with the pad. Note how IC1 pin 2 has a trace that is off the center of the pad. The trick in eagle is to always route starting at the pad. This gives you better alignment.
When routing, select the second routing tool - the one with 45 deg bends in it - to get automatic 45 deg angles.
Another thing to consider is grouping components. For example. R2 and R3 could be place side by side. Try rotating R2 90 degrees and placed next to R3 to see what I mean.
On the holes - have you tried a drill? Eagle supports up to something like 1/2".
Philba - thanks much for the detailed example - that is very clear. Let me go back and fix/improve the design. I will come back in a couple of days, hopefully with something better and neater
I found the HOLE tool, and I am now using that for the two holes that have no electrical connection. I also fixed the problem with the via drill size, by sligtly relaxing the design rule. I also redo many of the routing wires to make them more tidy as you guys recommended. Here is an updated/cleaned version:
