OK, here’s what I’m seeing at first glance:
thanks jwpartain1
what does " probably be NPTH ([e]dit>Pad type) " mean ?
apart from hole size do you think any thing else
Regards
He is suggesting that the pads labeled “Hole” in your footprint should NOT be “plated through”. He reminded you that this characteristic (“plated through” - PTH - versus “Not plated through” - NPTH) can be changed by editing the pad’s attributes.
To edit pad attributes, either:
- Hover the mouse cursor over the pad and press the “e” key; or
- Right-click on the pad and select “Properties” in the pop-up menu
You specify NPTH in the “Pad type” selection box.
“Plated through” (PTH) means that an electrically conductive connection is created between top and bottom layers of the board by depositing metal on the interior wall of the drilled hole. The metallic cylinder created by this plating process is sometimes called a “barrel”, or (rarely) an “eyelet”. The plated hole also provides a more secure mechanical attachment than an unplated hole. I believe plated-through holes started to replace mechanical eyelets in high-reliability and high-complexity electronics in the 1960’s, but since the 1980’s just about all commercially fabricated boards with two or more circuit layers have used plated-through holes to mechanically mount, and electrically connect, electronic components in a circuit assembly.
A “Not Plated Through Hole” (NPTH) does NOT provide electrical conduction between circuit layers. The walls of the hole are left in their natural drilled state. Are commonly used for the board mounting holes and for places where components attach to the board without electrical connection. Sometimes a pad is placed around the top or bottom of a NPTH to create a bearing surface for the mounting hardware, even though there is no electrical connectivity through the hole itself.
Dale
thanks for the detailed explained yes its good to have NTPH pad type as it is just a mounting hole.
i just did not follow this point from jwpartian1 “I usually like footprint origin to be centered for the part, SMT and TH (sometimes we use TH reflow or paste in hole processes here).”
and also as he mentioned holes size are slightly bigger but i feel its ok any way as extra space would be filled with copper
I’m not sure if this applies to Kicad, though I would guess it does. When you generate a .pos file from Kicad (File>Fab Outputs>Footprint position), which is the placement of all parts with the Normal+Insert attribute, it spits out xy placements from the origin of the component to the user placed origin for drill/place files. If this footprint origin is not the center of the component, there is some offset involved which the manufacturer’s pick and place machine cannot account for (without additional manual input).
Parts with centered origins ensure correct automated placement.
thanks jwpartian1
now i get what you trying to say but this footprint is centered as per the land pattern in the datasheet or am i missing something ?
or is it that you want the pin1 pad to be at the origin
Depending on your manufacturing process, it won’t matter for this part. You could be hand placing/soldering or hand placing/wave solder in which case, who cares where the origin is, I just mean as a best practice, your parts should have origin at the center of the entire component, like “it’s sitting in a rectangular hole on a reel, what’s the center of that rectangle?” kind of origin.
thanks jwpartian
now after you explained me this point " your parts should have origin at the center of the entire component"
that is when i got the idea it will be easy for the assembly house to place components
i have modified the file and placed it at the center for me it was just a matter of moving entire component to X,Y location
now can you please check if it correct ?
RJ45_TRANSFO.kicad_mod (3.6 KB)
Probably not. The current practice for the large majority of board fabricators says that the hole size specified on the drawing (actually, in the Excellon drill file) is the target size for the finished board - AFTER plating and finishing the hole. So if your drawing calls for a 1.78mm hole, the board fabricator will work to deliver a 1.78mm hole.
If you place an order for thousands of boards to be used in high volume production the board fabricator is likely to use the tooling he needs for creating a finished hole of the size you specify. Quick-turn prototype jobs (up to several hundred boards) will be manufactured using your supplier’s “standard tool rack”, unless you pay for something else. The standard tool rack contains tooling that produces hole sizes which the board fabricator believes are the most common or most useful sizes. The board fabricators I have used can all produce at least a dozen different hole sizes with their standard tooling, and some can do 25 or 30 standard hole sizes. Unfortunately, no two fabricators can agree on exactly which hole sizes are “standard”.
If your drawing calls for a hole size that is NOT one of the standard sizes, a quick-turn prototype shop will handle it in one of four ways:
He will INCREASE the hole size to the next LARGER size in his list of standard sizes. The boards you receive may have sloppy fits in all of the component holes, though it will hardly be noticeable for hand-assembly.
He will DECREASE the hole size to the next SMALLER size in his list of standard sizes. (This is rare.) The boards you receive may have tight fits in all of the component holes, and some may require an extra push to get a pin or lead through the hole.
He may round-off your hole size to the closest size in his standard list. Hopefully, you won’t notice the difference (especially if his standard tool rack has a good assortment of well-chosen sizes).
He may put your job on “hold”, until you send drawings that call for only the sizes on his standard list. This may be philosophically the most correct approach but it is very unpopular due to delays while information flows back and forth.
Of course all hole sizes are subject to manufacturing tolerances, typically several mils (0.1mm) or so.
Many quick-turn vendors tell you on their web site how they handle this problem. Or you may have to ask. Or select a preferred fabricator, determine what his standard hole sizes are, and make sure your footprint library uses ONLY those sizes. (Yeah, that means we create, organize, and maintain our own local libraries.) If a board fabricator changes a hole size he may, but probably will not, send an email telling you that he is doing this.
Dale
thanks pal
for a information on hole size it is better i stick to the datasheet hole size since i had taken it from the library hence assume it was almost correct size even i measured it
can some body please verify the bellow footprints
Pin_Header_Straight_1x06.kicad_mod (2.5 KB)
USB_A.kicad_mod (2.9 KB)
bellow is the datasheet for all 3 in sequence
http://www.cui.com/product/resource/pj-002a.pdf
http://datasheet.octopart.com/SSHS-123-D-02-GT-LF-Major-League-Electronics-datasheet-8326400.pdf
http://datasheet.octopart.com/87520-0010BLF-Areva-datasheet-13493241.pdf
Regards