How to make PCB footprints in Protel?

Hi
I am new to Protel, i want to create new footprints and for that somebody told me to read datasheet and you can make it.... but i dint exactly know whcih info to pick from datasheet and how could i use that info in Protel PCB footprints????

PCB Footprint

Mr Karesz,
you havnt answered my qs as far.... I am new to protel but have made fpga (MAX3232 footprint) ... actually i am trying to learn it first...
Now i want to check that the footprint which i have made is correct soo that i move on.. and if not then i make it again!!!

Added after 2 minutes:

Could any one please tell me step by step procedure of checking the footprints and then correcting it... if any thing went wrong!!!
Any lectures or websites would also be useful and of great help for me...

PCB Footprint

Hi,
Your welcome-of course!
Is it not easyer to give a "pdf/picture" of your footprint to see that as a description of dozen words pls?
1,
If you have to make a FP, check the datasheets for extrem tolerances & in detail pls!
They are often wrong drowed/constructed, some times you can correct the needed data with calculations, some time we must work with assumed data! :-(
2,
YOU MUST ALL DATA/MEASURES CONTROLL form your component-datasheet!!
Different vendors have often different measures, but referred to same packaging! :-(
3,
By SMD, SO16-W here; pad distance/pitch is exact to have (some ICs exists w. pitches of 0.635/0.65 & 0.5 mm too!) :-(
4,
Make the pad width (& length too) slightly bigger/more as the maximal pin width (yet 0.51mm), als i.e. 0.55-0.6mm.
5,
Work with a sortiment of pad/pattern collection with the time_so far as possible is!
Its very bad (later) if you will know never, is these yet 0.53 mm or 0.58? Tha you will find out, they has had i.e. a with if 0.55 mm....
6,
Solder maske (drow it every time with your footprints!); is i.e. 100um more to take as the patter/pad measures(so it have an higher measure pro side of ca. 50 um, enough for a good practicable vendor! It can/must be some time very tricsy by SMD regulators/pwr FETs for good solderability & less thermal problems in SMD oven, but its a speciality)
7,
Place every time a pick point on your component pls!
Your PCB montage will some cheaper if the partner for populating will become a data file and must not evaluate it from your PCB-design.
8,
Glue point = same as above, place it every time on your component pls!
Your PCB montage will some cheaper if the partner foe populating will become a data file and must not evaluate it from your PCB-design.
9,
Length of pads:
Calculate it from datasheets exterms=here are minimal internal distances of pins, but maximal lengt of pins to check!
10,
Outer distances/width of footprints; Your IC can measure 10,63mm also not less as i.e. 11.8mm= so will you have relative enough place for a fine soldertip for hand solderings too!
11,
The pad patterns place symmetricall_especially interesting by passives, in othercase will be the second pad not exactly on your raster_bad for connecting & DRC :-(...
12,
Drow every time a (TOP)silk for your components, what is equal with the MAXIMAL possible contures/measures of your phisical component!
It helps for you much by placing befor real routing the board!
13,
Do NEVER drow silks over pads/vias their you will have to solder!! Be care, that they have a separations distance of .e. 0.3mm from that.
14,
Have a library for only for you, added every time the newer components to that & import your components/elements from here into the design.
Some CADs can make it with a function(i.e. "archive"), will reduced from your library only
to the the used components/footprnts, but its every time very CAD specific...

So much after a little/speedy thinking...
Good luck!
K.

PCB Footprint

If you want to check the footprint you made is correct or not you can do one thing if you have the component available to you (MAX3232 in you case) than you can take the printout of the footprint created by you in 1:1 sacle and try putting the component on it and check if it matches or not.
Otherwise you can also get the footprint or the solder pattern(it is same as footprint) if you do little search on internet for the components.

PCB Footprint

Hi Ricky,
I think that the (from web & overall) collected footprints are the worsest possibility to work with systematic, professional - seriously!
At first you can not check the passability with a "put a component on the print out" methode....
Than; You have some tolerances of print + you dont forget the tolerances of components measures self from same producer, than the differences between different producer...
Otherweise you can not work so for a serious layout generation, OK: at home will it go too, but only for home/self used layouts pls!...
K.

PCB Footprint

Get the IPC footprint tool for footprint information.

It's free

PCB Footprint

Hi Karesz,

I only suggested him to get "internet collected" footprint to just check the footprint created by him is correct or not andif footprint provided by compnay itself, as per your comments, could be wrong than I dont think you will be trusting their datasheet either.
And for printout method I myself do that for the new packages and I assure you that I never had any problem in manufacturing for the same footprint and it worked not only for home PCBs but professional also.

Regards,
Ricky

PCB Footprint

Hi Ricky,
Dont worry, I will not try a personal attack, I told only, that these methode is not enough precise for professional checking.
I think you can agree with me?
You will have in all case problems by high pinout/fine pitch (0.5mm) packages, & what about i.e. FPGA`s pls?
Greetings!
K.

Re: PCB Footprint

Look at IPC-7351, calculators are free.