Very new to this, and concerned with getting it right. This is a transmitter module intended to remote control a hacked pushbutton. The datasheets for the Tx chip and antenna are here:
Operating notes: 3v power applied to the PWR jumper (not sure if I’ll actually put a jumper header there, or just solder in wires). A push-button is attached to the BTN jumper (same). When the pushbutton is pressed, current is sent to the PDN pin (1) and DATA pin (5), triggering a transmission. When the button is released, the Tx goes on power down.
The transistor, LED, and two resistors are for low-voltage indication. When the low voltage pin goes low, the voltage dropped below 2.1V.
One issue of concern is that the negative leg of the LED should just go to the ground plane, but I couldn’t get it to do that. So I drew a bottom-layer route from the LED to a spot on the ground plane. That worked, but there’s still a piece of rats-nest wire going from that spot to the left pin of the BTN jumper, is this a problem?
Also, the DRC keeps throwing distance and drill distance error on the two jumpers. I got them from the SFE library, is there a problem with them?
Finally: the antenna microstrip is supposed to be 50 Ohm. There’s a calculator for determining the proper width, but it requires me to know the dielectric constant and thickness of the board material and the thickness of the copper. Anyone happen to know these for the BatchPCB boards?
You actually don’t have a ground plane, and nothing is connected to ground. Click on the “name” tool (its a resistor with the name bolded) and click on the edge of the ground plane until the dotted line shows up. Rename it to “GND” and it will automatically connect to the ground pins. You should also make the traces thicker, for this you can use 12mil. Also, you didn’t ground the antenna.
Post the Eagle files and ile clean it up for you and look it over.
The plane is named GND, but I still couldn’t get it to connect to the pins like I thout it should. That why the via between the two jumpers should connect the plane to the gnu terminal, no?
Completely missed the need to ground the ant, oops…
I’ll post the eagle file when I get back to the computer, one question though - do I need to post the librar file, too or just the schematic and board?
Did you click the ratsnest button? the green net thing. I don’t need the library, just the brd and sch files. Eagle carries all the data you need in these files.
Yes, I clicked ratsnest (repeatedly…), but still no luck. Can’t seem to get the recomended trace for grounding the antenna, either. Files are attached.
Huge favor request: I appreciate you offering to clean up the pcb, but I’d like to learn what to do for next time. Can you let me know what (and how) you did, exactly, to make it better?
Not at all, its good that you want to learn as opposed to having other people do it for you.
I don’t know what headers you used, but they are just odd. If you search “header” in the dialogue when you type “add”, any of the normal sounding ones work great. The ones you had I think placed a hole over a via, essentially rendering the via useless. The ground plane would not cross the perceived edge of the hole.
Also, you Antenna library does not have all the ground pins mapped. You only have one ground pin connected, you need to map the other ones so they can be connected to ground. In your library, go to your symbol for the antenna and add 3 more pins. Go to the device, and connect the pads to these new pins. In the schematic, ground these 3 other pins. On the Board, Copy the GND Via connected to the second pin of the antenna, and place it near the other 3 ground pins. Route them.
I also re sized the dimensions to make it symmetrical, and rearranged the components. It is standard practice to only use 90, 180, and 45 degree angles. There is nearly never a use for Eagle’s straight line routing option.
Are you familiar with Eagle’s DRC? Type DRC, and a dialogue pops up. All these options can stay the same until you get to more complex PCB’s, but the Dimension setting (i.e. no copper within x distance from a edge) is a bit large at 40mil. You can change that to 15 mil. Also, under the masks tab, there is an option called limit. This creates a stop mask for everything over this dimension. I set this to 32mil, as the vias are 32 mil. Now the via’s will be covered with solder mask and insulated.
Ask if you have anymore questions!
Another note: Never use traces bigger then the pads themselves, especially when directly connected.
rp181:
I don’t know what headers you used, but they are just odd. If you search “header” in the dialogue when you type “add”, any of the normal sounding ones work great. The ones you had I think placed a hole over a via, essentially rendering the via useless. The ground plane would not cross the perceived edge of the hole.
Don’t know - something from the SFE library… Changed them out, worked great.
Also, you Antenna library does not have all the ground pins mapped. You only have one ground pin connected, you need to map the other ones so they can be connected to ground. In your library, go to your symbol for the antenna and add 3 more pins. Go to the device, and connect the pads to these new pins. In the schematic, ground these 3 other pins. On the Board, Copy the GND Via connected to the second pin of the antenna, and place it near the other 3 ground pins. Route them.
Ah. Was hoping to avoid needing 4 unnecessary pins in the schematic, but I guess there’s no way around it. Fixed.
Another note: Never use traces bigger then the pads themselves, especially when directly connected.
I’m assuming you mean the antenna line? The DS says to use a 50 Ohm line, and that for standard pcb materials, that’s 111 mil wide. Not sure what the characteristics are for the BatchPCB boards, but 111 mils is way wider than the actual pads…
One more note - the chip ds says no traces under the tx chip, so have to route around it…
Anyway, here’s another attempt - I didn’t use the one you sent, just used the info you provided to re-do the board from scratch. Let me know what you think.
Good points, I only skimmed the datasheet. What I would do for the 50ohm line then is to use the size that is on there, bring it out a little, then widen the trace once it clears the pad.
Other then that, it looks good.
The upcoming release of eagle aims to make it so you can connect multiple pads to one schematic pin, which will help tons.
I would move the right dimension line in, to make it equal. Also, I would remove the silkscreen from under the part, the part will not lie flat. This is important especially since it is a component with pads underneath. Try to give each gnd pad on the antenna its own ground via. Move the left via to the left side of the pad and the right via to the right side. Then each can have its own.
