today my pcb maker told me they can't get all components on the board. I was wondering if some might have suggestions for improvement. Attached the schematics and pcb design. the part outside the white lines does not fit on the board. pcb size is 15x8mm. Total available space for pcba is 15x8x6mm. i appreciate your help.
In reply to clausule:
Either one of two things has to happen here.
1. The board size needs to increase or
2. The component count needs to decrease.
Simple as that.
A lot of the microcontrollers today have an internal RC oscillator that can be used in place of an external crystal / oscillator. You may want to look into using the internal clock source and verify it can provide the stability required to support the USB comm. Also, I think you can remove the diode in the reset line or at least go with a much smaller part. Making these two mods will free up some board space, but I stiil don't think you will get everything in the given area.
Another thing, look into the actual size of the parts vs the silk screen around them. A lot of room is being taken up by the silkscreen. You'll notice that a lot of the high density boards eliminate silk from the design which allows for closer placement (within DFM constraints). But your board design provider should be aware of all of this.........
In reply to TH Designs:
If you have the room for another pcb in the enclosure, that might work well. Maybe put the USB conn on its own board and that would free up a lot of room for the micro and LEDs on another board.
It usually never works out well when the mechanical design is done before the electrical / board design. But I run into this all the time.............
Not sure how practical any of these suggestions might be given the number of unknowns in your situation, but they've got to be more feasible than having parts hanging off of the board. This might not get you to where you need to be, but it might help:
1) Drop the silkscreen. Refer to an assembly document for placement info. You don't have room for ink.
2) Reduce case sizes for passives. Hard to tell from the screen capture, but if your manufacturing house/ assembly person supports it, use 0201 components where possible (if you aren't already). I'm going to assume 01005 case sizes are not supported in your situation.
3) There's a 10 pin device that looks like a USB connector - I don't see it on the schematic, maybe some pins aren't shown on J5 in the schematic? Regardless, if it is a USB connector, make sure you are using the smallest connector possible (micro-USB). If a different size connector (standard USB or mini-USB) is required for whatever this thing will interface with, make an adapter outside the box.
4) For the 10 pin device mentioned in #3, see if you can find a version of the connector without thru-hole pins to pick up a little bit of space on the back side. I think they exist, although you may sacrifice mechanical robustness if you make the swap.
5) I see 2 sets of 3 LEDs - do they report information simultaneously or can their functions be combined? Use 3 LEDs with a slow blink for function 1, fast blink for function 2? Or, use 4 LEDs - 1 to indicate either function 1 or 2, use the remaining 3 as already planned.
6) Is there room in the enclosure in the z dimension? If so, maybe add a header/b2b to bring signals off the original board onto a sub board that could house the switch, LEDs, etc.
7) Instead of placing both C6 and C11, only put 1 of those components in your schematic. Put a note in your schematic indicating both values are required. Hand place second cap directly on top of first cap after boards are built.
Hope this helps. Good luck.
In reply to mfris:
1) will ask them to drop it tomorrow!
2) my pcb maker is in china and they have access to all components. why you assume 01005 is not suitable in my situation?
3) we dont have 10 pin device. we have a micro-usb connector JAE DX4 series with 5 pins (in schematics only 4 pins shown as we dont need the pin for 'usb to go', need to tell pcb maker to leave 5th out right?). And we have 5 pins to solder wires on for pickit2.
4) for micro-usb connector i will make sure they use the smd version.
5) there are two LEDs, one on each side. Both are the same, RGB LED with 6 pins
6) i need to check that. I think now we have PCB 1mm + micro-usb connector 2.35mm (highest component) so 3.35mm. I'm not sure if he uses both sides of the PCB though... he said he did but my programmer said he didnt... im confused.. we also have a switch and i told them to use any switch they want as long as it fits. for reference i gave them datasheet of OMRON B3U smt tactile switch 1.2x3x2.5mm (HxWxD), comes in all angles. If the switch is on the same side as the micro-usb connector we could keep 3.35mm or max. 4mm. The PCBA housing is (without the reserved space for LEDs, these are not fixed on the board!) 15x8x6mm. So we would have around 2mm left in z dimensions i guess. what can we do with this? micro-usb connector can be anywhere on z axis so we are quite flexible... Last resort would be 2 PCBs right?
7) this step i dont understand. you mean use one smd at the bottom and one through hole on top?
We already decided to replace the diode with 1k resistor (0805 or 0603, should i go for dimensions mentioned in step 2?) and replace the crystal with a Murata CSTCE-G 12mhz resonator.
You think we can make it fit with all these steps?
For item 2, if cost is not an issue and your manufacturing solution supports it, you should use the lowest case size feasible. For capacitors, you should confirm that capacitance, tolerance, and appropriate voltage rating are supported in the smaller case size. For resistors, you should confirm the power rating and tolerance is sufficient for the smaller case size .
For item 3, you should follow the component vendor's recommendation for footprint - all pins should have a pad on the board, even if they are not being used in the design.
For item 7, I was suggesting that you delete either C6 or C11 in your schematic so that you only have to place one component on that net in your PCB editor. After the boards are assembled, manually solder the missing capacitor directly on top of the placed capacitor so that the 2 capacitors are touching each other, with 1 capacitor sitting directly on top of the other on the same side of the board. That was a suggestion to help you work through tight placement constraints on a small, prototype build. It would not be practical/feasible on a larger scale production run.
It's hard to say if these steps are sufficient to get you to where you need to be, or if you can get to where you need with only some of the suggestions without actually sitting in front of the CAD tool making the changes.
Have you tried piggyback soldering for discrete components ?