How do I create a ground plane in eagle?

Thread Starter

magnet18

Joined Dec 22, 2010
1,227
Right now, I'm clicking the "draw a polygon button", changing isolate to something other than 0, then drawing a box around the whole board (which appears as a dotted line), then renaming the polygon to GND (Same name as my ground plane), and it won't fill in!
Any help?? :(
 

SgtWookie

Joined Jul 17, 2007
22,210
Did you click Ratsnest?

That's usually how you fill them.

Make certain that the polygon width is >0. I use 10 mils.

I usually set Isolate to 16 mils/0.016", and spacing to 50 mils (same as grid).

If you're doing the entire ground plane, set Rank higher than 1. Otherwise, if you want to create a small polygon in the middle of the ground plane, the ground plane will cover it over. Rank 1 means it's the boss. If you give it a higher number, it won't overlay ranks that are lower.
 
Last edited:

SgtWookie

Joined Jul 17, 2007
22,210
It's not intuitive.

I keep forgetting how to clear the polygon for when I want to move traces around. You can use the Ripup command, and click on the polygon edge; just inside it. Make sure the polygon edge is the closest thing to where you click ripup, or you'll rip something else up.

[eta]

The RIPUP command changes routed wires (tracks) into airwires. That can be done for:
  • all signals (RIPUP;)
  • all signals except certain ones (e.g. RIPUP ! GND VCC;)
  • one or more signals (e.g. RIPUP D0 D1 D2;)
  • certain segments (chosen with one or more mouse clicks)
  • all polygons (RIPUP @;)
  • all polygons of certain signals (e.g. RIPUP @ GND VCC;)
  • all polygons except those of certain signals (e.g. RIPUP @ ! GND VCC;)
 

Thread Starter

magnet18

Joined Dec 22, 2010
1,227
Thanks, I didn't know about the ! operator

Alright, I've attached what I've got, but is there a way to make the isolation larger for just one certain net (the +180V)?

(I also attached an avatar for you... so you can join in the festivities
Use it if you want :))
 

Attachments

Thread Starter

magnet18

Joined Dec 22, 2010
1,227
Whoops, apparently I attached the wrong file :p
Here it is

[EDIT]
That's weird, whenever I save it, it doesn't save the planes, and I have to hit ratsnest again to make them fill :confused:

Anyone know how to fix this?
 

Attachments

SgtWookie

Joined Jul 17, 2007
22,210
Thanks for the thought with the red thing on top, but I don't do the "unauthorized headgear" thing with a uniform. ;)

I got lost in the details with your board; traces desperately needed some fattening up.

I don't know for sure what's HV and what's LV, as you didn't NAME your signals other than the defaults - so anyway, look at the attached (don't overwrite your original though)
 

Attachments

Thread Starter

magnet18

Joined Dec 22, 2010
1,227
Thanks for the thought with the red thing on top, but I don't do the "unauthorized headgear" thing with a uniform. ;)
Lamesauce :p

I got lost in the details with your board; traces desperately needed some fattening up.

I don't know for sure what's HV and what's LV, as you didn't NAME your signals other than the defaults - so anyway, look at the attached (don't overwrite your original though)
Thankyou Muchly, You saved me a load of work :D
I edited some DRC errors, woulda done it at school, but they recently banned personal laptops, because they can have unrestricted access to the network, even though I can have unrestriced access to the network at home through the VPN... incompetence :p
Now I'm waiting for my parents to finish getting their hair cut, stealing their interwebs (not really stealing)

But I digress, does everything look good?
 

Attachments

SgtWookie

Joined Jul 17, 2007
22,210
Upload your .sch file as well. I don't like working on just one of the files, as if they get out of sync, you'll have a mess on your hands.

Also, unless the wires have meaningful names assigned to them, I will have no idea what kind of signals are on them - except for a few, of course.
 

Thread Starter

magnet18

Joined Dec 22, 2010
1,227
Upload your .sch file as well. I don't like working on just one of the files, as if they get out of sync, you'll have a mess on your hands.

Also, unless the wires have meaningful names assigned to them, I will have no idea what kind of signals are on them - except for a few, of course.
I uploaded it, sorry bout the manes, I'll work on that, the highish voltage is the nets on either side of the uf4007
 

Attachments

SgtWookie

Joined Jul 17, 2007
22,210
There are 29 consistency errors between the schematic you uploaded and the board I'd uploaded.

What's going on?

I guess you made a bunch of changes in the schematic without letting me know about it. So, what I have here is worthless.

Upload a matched pair of schematic/board.
 

Thread Starter

magnet18

Joined Dec 22, 2010
1,227
What? I didn't make any changes to the schematic at all?
Especially not 29, I would remember that...
[EDIT]
OH, I remember now, I changed the name of the ground net in the board, if you change it back to GND it should work, sorry bout that :(
 
Last edited:

SgtWookie

Joined Jul 17, 2007
22,210
Here you go. I'm kind of tired of fiddling with it.

You have lots of long traces for reasons I don't know - possibly due to how it fits in with other boards. If you had flexibility in where you could put things, the board could be made a lot smaller - and as you probably know, board real estate = $$$.

I revised the schematic so that it was easier to read. You really had things packed all together, and names/values overlapping everywhere so they could not be read.

I don't like excessive of white space - you do need some in there though; otherwise it's just too difficult to read.

One of the first things you should do when creating a schematic is to drop in a frame. Open frames.lbr, select one and drop it in there, with the lower left corner over the "+", which is the 0,0 point. If you don't use 0.0 for your starting reference point, your printouts can look whacky; you might get multi-page printouts for what seems like no reason.

Starting with an A size frame, either portrait or landscape, is good. That'll fit one 8-1/2" x 11" page. You can always choose a larger frame later if needed; but without one it's easy to lose track of where you are.

Your R61 and R71 were too small at 1K. The minimum value you should use for R1 in a typical R1/R2/C1 555 astable multivibrator configuration is 100 Ohms per volt of Vcc, or the pin 7 current becomes excessive. I increased them both to 1.2k. Impact on frequency and PWM% will be minimal. If you want to have a duty cycle that is less than 50%, use a diode across R2 (in your schematics' case, that's R62 and R72) and increase R1 (R61, R71).

Your R70 and R77 are far too large, and R69 and R76 are WAY too small. I don't know why you did that. This should be a "fine tune" for the HV adjust, not an adjustment from 45v to 9.8kV :eek:

Try changing the pot from 10k to 1k, and the fixed resistor to 1.5k. You may need to adjust the values a bit to get a ~10% adjustment range, but you really do not want a very wide range; it's not necessary, and it could wind up damaging Nixie tubes.

I suggest that you strongly consider replacing the IRF840 MOSFETs with IRF620's. This will limit the maximum output to 200v, as the body diode is avalanche rated for that. It would be better to risk burning up MOSFETs than the Nixie tubes; as MOSFETs are cheap and plentiful.

I added a couple of test points for checking the high voltage, but in the voltage divider.
 

Attachments

Thread Starter

magnet18

Joined Dec 22, 2010
1,227
Here you go. I'm kind of tired of fiddling with it.
In that case, I thank you doubly
You have lots of long traces for reasons I don't know - possibly due to how it fits in with other boards. If you had flexibility in where you could put things, the board could be made a lot smaller - and as you probably know, board real estate = $$$.

I revised the schematic so that it was easier to read. You really had things packed all together, and names/values overlapping everywhere so they could not be read.

I don't like excessive of white space - you do need some in there though; otherwise it's just too difficult to read.

One of the first things you should do when creating a schematic is to drop in a frame. Open frames.lbr, select one and drop it in there, with the lower left corner over the "+", which is the 0,0 point. If you don't use 0.0 for your starting reference point, your printouts can look whacky; you might get multi-page printouts for what seems like no reason.

Starting with an A size frame, either portrait or landscape, is good. That'll fit one 8-1/2" x 11" page. You can always choose a larger frame later if needed; but without one it's easy to lose track of where you are.

Your R61 and R71 were too small at 1K. The minimum value you should use for R1 in a typical R1/R2/C1 555 astable multivibrator configuration is 100 Ohms per volt of Vcc, or the pin 7 current becomes excessive. I increased them both to 1.2k. Impact on frequency and PWM% will be minimal. If you want to have a duty cycle that is less than 50%, use a diode across R2 (in your schematics' case, that's R62 and R72) and increase R1 (R61, R71).

Your R70 and R77 are far too large, and R69 and R76 are WAY too small. I don't know why you did that. This should be a "fine tune" for the HV adjust, not an adjustment from 45v to 9.8kV :eek:

Try changing the pot from 10k to 1k, and the fixed resistor to 1.5k. You may need to adjust the values a bit to get a ~10% adjustment range, but you really do not want a very wide range; it's not necessary, and it could wind up damaging Nixie tubes.

I suggest that you strongly consider replacing the IRF840 MOSFETs with IRF620's. This will limit the maximum output to 200v, as the body diode is avalanche rated for that. It would be better to risk burning up MOSFETs than the Nixie tubes; as MOSFETs are cheap and plentiful.

I added a couple of test points for checking the high voltage, but in the voltage divider.
Thanks for the schematic tips and the MOSFET tip, as for the resistors, I knew it worked, so I didn't worry about it, I'll change it though.

I really doubt the circuit could get up above a few hundred volts, but that could damage the tubes, and it never hurts to be safe I guess.

Thanks!!
 

SgtWookie

Joined Jul 17, 2007
22,210
I didn't explain about changing V+ to VCC, and moving V+ to the right of the switch.

The 555 timers you are using have V+ for their positive supply. You'd used V+ on the side before the switch, but also had connected the timers' V+ to the node (I think it was N$118) that was the trace after the switch. That creates a conflict in Eagle; by default it connects everything in the board with the same signal name using air wires - but V+ on the timers and V+ on the input wire were supposed to be different nodes.

That's why I moved V+ to the right side of the switch, as it resolved the conflict.

You have IP1, the 10-pin dual jumper header, locked in position - why, I'm not sure; perhaps it needs to be there for connecting to another board. The current routing of HV2 gets very close to the edge of the board. It would be preferable to keep it further away from the edge. The easiest way to do that would be to reassign the pins for HV1 and HV2; simply exchange them in the schematics. Otherwise, you'd have to send one of the signals to the bottom of the board and back up to the top layer so they could cross each other.

I scattered a number of vias around to connect the two ground planes together.

I took care of most of the overlapping names and values; but I missed a few. D11 in the upper right hand corner is one. C22's value field is misplaced above D2 (2.2uF). I forgot to move all of the reference designators (NAMEs) out from under components; it's OK to hide the value under a part, but not the name/reference designator.

You still have a lot of resistors with minimum radius bends in the leads - like R61, R62, R66 in the lower left corner. You usually want to avoid that, as it is difficult to bend the resistor leads that close to the resistor body without putting stress on the body; that can lead to mechanical failure. With the vast expanses of unpopulated areas on this board, there is no reason to use resistors with the shortest leads possible. If you're planning on using 1/10 W resistors (you could for most of them) then you should change the package to indicate the actual size of the resistors being used.
 

Thread Starter

magnet18

Joined Dec 22, 2010
1,227
As far as the high voltage SMPS supply - you didn't give me any feedback if items were in a specific location for a reason, or if they could be moved around. That board could be made quite a bit smaller if you had flexibility in where things could be located; like I/O connectors, lights, etc.
Well, the header is in a good place to connect to the other boards, but if it was rotated and moved to the left side of the board it would still work well

the lights and switch can be moved around, but it would probably be best if they stayed towards the top of the board, and the power connectors definitely need to stay up there (towards the center of the clock)
The only way around that would be to move everything to he bottom, that would allow the board to be positioned on the other side of the clock

other than those things, just about everything can be moved. I just layed it out the way that made the most sense to a human. For some reason I love to see boards where the logic flow just makes sense when looked at, not running randomly everywhere.

Thanks for fixing the power by the way, I wouldn't have caught that

and I was planning on using 1/4 watt resistors, I wasn't sure how much power was flowing and just went with what worked IRL (the small bends and everything)

also, for the record, this was the first board I ever layed out :p
 

SgtWookie

Joined Jul 17, 2007
22,210
Speaking of the power connectors - did you make those yourself, or did you happen to download them from somewhere?

I don't have "power connector.lbr" - please upload it. There are some odd things about it that need to be rectified. Rename it as "power connector.lbr.txt" before uploading it.

Do you have a datasheet for the actual power connector that you are planning on using? If so, will you post a link to it?
 

SgtWookie

Joined Jul 17, 2007
22,210
Here's a go-round at a remake.

I ripped up everything, basically left the placement of components along the top alone except for some misc. alignment, moved the switch from left to right, and then basically moved everything up and closer together.

C9 and C12 weren't really doing anything important that I could see; they aren't routed. What IS needed is a couple of 100uF-330uF caps next to L1 and L2 on the 12v trace.

The board was 4"x3.2" before I started; I left it that size so you can see how much smaller it will be.

I don't know why you had three groups of three LEDs. I removed the center group, as they were preventing locating the HV traces together. Now all of the HV stuff is pretty close together towards the middle of the board, and traces to the connector are relatively short.
 

Attachments

Top