[Discussion] How do you Check your Footprint in an easiest way?

As i wrote in the title, In this thread, i want to discuss about how do you check your footprint?

Footprint Creating seems to be the job that you can do easily, but it's one of the most important things that need to do perfectly, if there is any mistake, you know what i mean ... :-(

Normally, I do it visually by comparing the footprint with the datasheet of Parts, but sometimes i make a mistake. How about you guys?

Thanks!

I check that others have made footprints very often.
I use a really long checklist - it has over 85 checks on it.
I am expected to tick or comment on every one of them - what a PITA that is!!

But it does remind me what to check for and can catch some things that I forget.

For consistancy:
I use a spreadsheet for every bit of a part, symbol & component - this specifies what lines, text sizes etc are to be used.
This gives me something to check against.

The components I check are usually made to the IPC7351 component standard and using the pcblibraries footprint\library wizard, this is done by entering the component dimensions into the tool.
I could re enter them but this is a PITA too, I measure distances match the datasheet, if I'm finding it a little hard then I recreate the component itself in 2D with lines\boxes and can place it over the footprint to see if it fits - this generates a "it will do" lol. If I can get a 3D model of the component I whip it into Inventor, create a sketch of it top view & save it as DXF then import that - this is especially useful with connectors.

The main thing I use when checking is my brain, I think about what the items are being used for and how they will be assembled, soldered, repaired etc to consider if its all OK.
This is the bit that finds the most issues

Checking takes me longer than it would take me to make them in the first place.

Mistakes do happen - we are human not robots, even when we have PITA check lists.

Hi,

Yes a checklist helps a lot, especially when you have some "company" specials in your libraries.

Some standard info:
https://www.edaboard.com/threads/128769/

For an rough optical check I print out 1:1 and put the device on it. No precise test, but you may find some issues.

Klaus

Mattylad said:

I use a really long checklist - it has over 85 checks on it.
I am expected to tick or comment on every one of them - what a PITA that is!!

Click to expand...

Wow, i have the checklist with about 20 categories, and i have alot of things to do.

I've been thinking about create a tool to help me to do this job, but it seems like impossible

Beside, i will consider about the IPC Standard, but most of the datasheets have the recommended Layout for the chips, and to make sure that Components work as designed, create footprint following the recommended pattern should be put in consideration.

Thanks for replying

Jack

My checklist covers symbol, component and footprint so not all 80+ checks are for the component.


There is a vast difference between the manufacturers recommended footprint layout and what a component actually needs, many of the manufacturers layouts are ancient and overkill.
If you put the manufacturers layout in your library for every component you are going to end up with multiple copies of the same type of footprint, SOT-23 is an example - why have one for each manufacturer when the component is a gnats kneecap different and would all fit on one footprint for all.
Manufacturers recommendations are also not standardized, IMO your best bet would be to use the library tool from pcblibraries.com and create them to IPC-7351C.

JackSanji said:

Wow, i have the checklist with about 20 categories, and i have alot of things to do.

I've been thinking about create a tool to help me to do this job, but it seems like impossible

Beside, i will consider about the IPC Standard, but most of the datasheets have the recommended Layout for the chips, and to make sure that Components work as designed, create footprint following the recommended pattern should be put in consideration.

Thanks for replying

Jack

Click to expand...

Use IPC footprints as your first choice always... These footprints have been tested and developed within the industry, have been used and tested on thousands of boards and assembled in their millions. They work... Footprints from data sheets are secondary to the IPC-7351 standard and for all standard footprints (SOTs SONs SOT23s etc) I always use the standard footprint that is in my library. For the more esoteric footprints I use the dimensions from the data sheet then make it up as I go along... But then I have an intimate knowledge of PCB assembly from actually soldering the boards and working very closely with production departments for many years, so I know what is required. You can also get a better understanding by reading some of the stuff on IPC-7351, CAD libraries and IPC specs to get an idea of what a solder joint is, how it is formed etc. etc. Its all part of the skillset required to be a PCB designer, if your boards cant be assembles reliably then you will have problems.


And as Matt said and I demand, oly one SOT23 footprint per library, anymore is wrong.

As to checking, start with an exact size drawing of the component on an assembly layer (not every detail) and then it will be obvious if things are wrong. Getting drawings from manufacturers helps as well especially DXF and 3D data that can be also used to check the footprints, either by inporting the data or using IDF or step to place a 3D model on the footprint you have created.

Valor tool from mentor graphics can really do wonder in footprint checking . But the tool is costly and not affordable in many cases . They are updating the their valor library frequently or even create custom part on demand. ODB++ file from the PCB will be compared with the valor library parts and will report if any footprint mismatch with the BOM and PCB.

when ever DXF file for the component is available , especially for connectors , I used to import them in to a documentation layer while library creation. It helped for easy visual checking , like whether all the pins are in position , component outline dimensions etc.
now a days many tools support STEP file import also , this one is also can be made visual inspection easy.
IPC footprint generators are also available for popular CAD software's . LP calculator is one example.
" Tom Hausherr" had made excellent documents and tools for footprint creation.
http://www.pcblibraries.com/
**broken link removed**

marce said:

And as Matt said and I demand, oly one SOT23 footprint per library, anymore is wrong.

Click to expand...

Yeah, I'm considering to make my own Library, where each package has only one footprint, and also make it is the common Lib for my team

Toms tool is excellent for making footprints, especially as it's free for single use at a time.
Although there can be no substitute for learning to make them in your own CAD package.
Having a specification or guide is IMO essential to making consistent components.