Matrix PIC fix for v9 and v10 systems

Sorry, running late today so I've only just had chance to take another look.

Probably best to take this step by step as a lot needs to be done to the silkscreen.

We will get the pads and diode out of the way first:

Right click each package on the bottom row of the PCB (pads and diode) then properties and then tick smash.
Right click every name attribute and value attribute for each package then properties and change option display to off to get rid off them.
Right click every text label that you have added then properties and change the font to vector and the size to 40mil and 15%.
Move each text label so that it is at least 6mil away from it's respective package. Somewhere between 9-12mil is ideal to be on the safe side otherwise some of the text can be slightly cut off depending on the manufacturers capabilities.

If you can do the same for any of the other packages then that would be great although the method may differ for some like the resistors and caps where you would want to keep the name attribute and get rid of the other text/attribute. I will add this to the list though anyway so no rush if not.

I'll continue the list ASAP as I'm limited on time today.

 

...ok so now on to the resistors, cap and PIC:

Right click each package (resistors, cap and PIC) then properties and then tick smash.
Right click every value attribute for each package then properties and change option display to off to get rid off them.
Right click every name attribute then properties and change the font to vector and the size to 40mil and 15%.
Optionally change the name attribute of the PIC to "U1"
Delete every text label that you have added for the resistors, cap and PIC.
Right click "Comsoft v4 fix" text then properties and change the font to vector and the ratio to 15% then move the text so that it is centered again.
Optionally change to schematic and swap R1 and R2 names to make the numbering on the PCB more orderly.
Move each text label so that it is at least 6mil away from it's respective package. Somewhere between 9-12mil is ideal to be on the safe side otherwise some of the text can be slightly cut off depending on the manufacturers capabilities.

That way is slightly different than the pads and diode but could also have been used with them in which case you would have just deleted the text that you added and kept the name attribute instead.

Oh nearly forgot the Gnd pad. You can use either method for that, keep the text and get rid of the name or vice versa and then also change the font, size and ratio then move it 9-12mil away from the package.

One other thing is that whoever made that SO8 package seems to have added the pins on the tPlace layer rather than the tDocu layer which it should be. You will need to correct this before exporting the gerber files by:

Right clicking the package then open package, now right click every grey rectangle on top of the pads then properties and change the layer to tDocu. Once done make sure that you save the package and then go back to the PCB and then click "Update all" in the Library options of the menu bar.

It should look similar to this now:


I wouldn't personally bother adding a Gnd pour on a board this small and simple but if you do then you will also need to add some design rules so that you end up with the correct clearance from the edges of the PCB, usually about 10mil.

 

Will skip the ground pour idea, I think I finally got it. Looks very similar to what you came up with. Files are attached.

Maybe I can come up with a through hole design to use up some of my 1/8w 1.5k ohm resistors. This way is people want through-hole or smd either is a choice.

Thanks for the help and advice kel,
HaloSlayer255

 

Looks good. There are some issues with the board and schematic not being consistent with each other, some small routing issues and R1 silkscreen is a little closer than the rest but nothing that would cause any problems with the functionality of the board and if you went for it as is then the generated gerber files would be fine.

 

Alright sounds good, will try to see if I can pin down the issue in the schematic. Will probably go with 5 boards just need to get some money saved up and that might be a while. Since this is all smd, could I try using toner transfer on a few copper panels as a test run?

 

It's not worth it these days to spend time and effort etching your own boards when places like OSHpark will do 3 of these boards for just $5 with free shipping IIRC or places like PCBway and Seeedstudio will do 10 for $5 or less plus shipping. The parts wouldn't come to much either and if you're in the US then if I'm not mistaken Digikey and Mouser have free shipping also. So if you use OSHpark and let's say Digikey you should be able to make 3 boards for about $10 give or take. If you are not in the US then you might have to shop around to get the best deals on shipping.

 

Holy cow didn't know it was that cheap now a days. Will probably go that route since I'm in the US. I might be able to reuse the existing 12c508a pic chips if I form the legs carefully. Will probably check the cost for a batch of 10 then, plus the components.

Cheers Kel! (Kampai!)