• Welcome to our site! Electro Tech is an online community (with over 170,000 members) who enjoy talking about and building electronic circuits, projects and gadgets. To participate you need to register. Registration is free. Click here to register now.

Eagle footprint

Status
Not open for further replies.

Wilksey

Member
Hi Folks,

Does anybody have or would be kind enough to create a footprint for the Cinterion BGS2 value GPRS module?

It is an LGA arrangement and I am fine creating the device symbol, but I have no clue how to draw the footprint, I have read loads of tutorials and I just cant seem to line everything up etc. I am not even confident the pad sizes are correct, trouble is with through hole stuff I can print the footprint out and poke the legs through the holes and see if it is correct with some SMD stuff I can line it up, but LGA type stuff I can't see the pads as they are underneath the chip!

Any help appreciated!

I do have a datasheet somewhere I can send to someone if they are willing to help.

You can probably tell by the title but i'm attempting this in Eagle.

Many thanks!

Wilksey
 

jpanhalt

Well-Known Member
Most Helpful Member
Can you provide a link to a dimensioned drawing for the exact LGA that you need? Be sure it includes any heat sink areas.

John
 

jpanhalt

Well-Known Member
Most Helpful Member
I should have asked before, are you using Eagle 5.11 (or any 5.xx) or 6.0/6.1? I assume there is backward compatibility, but there is no need to make it more complicated than needed. I have both versions.

John

Edit: One more detail. will the solder paste stencil be 150 micron or 110 micron thick? The pads at 110 micron are 2.36X0.7 mm and at 110 micron are 1.75X0.7 mm. The thicker stencil allows more solder paste, so adjustment is apparently made in the pad length. My guess is that a bigger pad with a thicker stencil might lead to shorts. (The only LGA similar type device I have done was an accelerometer that I hand soldered...it only had 8 pads.)
 
Last edited:

Wilksey

Member
Hi,

I am using Eagle 6.1 free version.

I honestly don't know regarding the paste, there is a video from Cinterion on youtube of hand soldering the device, the PCB house I use normally deals with assembly work.

I guess the longer the pad the better for hand soldering with Cinterion's tinning method.

Thanks

Wilksey
 

jpanhalt

Well-Known Member
Most Helpful Member
I have a draft with the shorter length. Changing to the longer length is not a problem. Notice the spacing around the RF pad is a little different. Again, that can be dealt with. I ended up using two grids (1.2 and 1.0) with a minimum of 0.05 to accommodate the RF pad. (I may change my mind on that depending on the "BIG" problem described below.)

There is one BIG problem, as best I can see it. The drawing is not fully dimensioned. The inner ground pads were easy to do, because the corner distance (i.e., C/L horizontal to C/L vertical) is shown. It is 2 mm. I cannot find any way to relate the vertical outer pads to the horizontal outer pads.

If you can find it (no guessing!), let me know. I was following the recommended pattern(s) in Figures 45 and 46. I just reread it. I will redo according to Figure 44, which is fully dimensioned, and leave the stencil until later.

John
 
Last edited:

Wilksey

Member
Hi John,

I am terrible at reading dimension drawings I get muddled with the numbers and which bit they are referring to!

I would really like to be able to create my own reliable footprints from the datasheets, but can't seem to find any good information on how to read the dimensions correctly, do you have any pointers?

I hadn't actually noticed the distance difference between the RF pad and the normal pads, is it 1.2 for normal and 1.35 for the RF pads? I guess those are in mm units?

What is the stencil for? Isn't that for the assembly part? Or is it to do with something else also?

What is the corner distance? I can see 2mm between the two centres of the inner ground pads on figure 44. Is that what you were referring to? I don't know what C/L is.

Is the spacing between horizontal and vertical 2.5mm? From centre of the horizontal to the bottom of the vertical?

How long does it generally take to create a footprint from a datasheet of that complexity?

I wouldn't mind having a go myself but there are too many dimensions confuse!

Thanks again for your help!

Wilksey
 

jpanhalt

Well-Known Member
Most Helpful Member
I have a rough draft of the package to send you. There are a few additions I will need to make after reading the data sheet some more. It will probably be best if I also make the symbol and connect the pins too. If you have already made the symbol, please post it here. Since I had started with Eagle 5.11, I stayed in 5.11 for this draft. I plan to convert everything to 6.0/6.1 for the final device. 6.1 has a nice tool for measuring, which will make checking the dimensions much easier than doing it the 5.11 way.

I have never tried to send single devices from a library. So, let's see how this works. I made a separate library called TempETO. You will want to make your own personal library, if you have not done that already.

I zipped the file, since .lbr is not supported here. You will need to unzip and copy to your Eagle library. In XP, you can probably just move it using explorer. Alternatively, within Eagle, you can use Control Panel to make a new library.

Eagle has some ways to copy libraries, but I am rusty at that. I usually just open the object, select all, cut (or copy group for 6.1). Then in library mode, click on package and enter the new package you want to transfer. Eagle will not find it and will ask if you want to create a new package. Click yes. You will get a black screen. Under View, select grid, and make it what you want. In this case, make it 1mm for major (count =1) and 0.05 mm for minor. Then paste.

As mentioned, I used two grids (1.0 mm and 1.2 mm with the minor at 0.05 for both) . In general that is a bad idea with Eagle. However, in this case, the 1.2 mm grid made it easy to get the signal pads centered. Since the fine divisions were the same, it did not create a problem.

Now let's assume you forget to change the grid before pasting. The default will probably be in inches. There is no way you will easily get this package to line up with that grid. Play with it, if you want. But then just delete and start over with the proper grid.

I named the package LGA66 for the number of pins. If there is another name you prefer, let me know.

What is your time frame for getting this done? Depending on weather, I have some outside chores that must get done if it doesn't rain. In that case, I won't be able to get back to this until tomorrow afternoon. I am on Eastern Daylight time, USA (GMT-5?).

John

PS, Those extra lines in Dimension layer were used as drawing aids. They will be deleted in the final version.

View attachment 62574
 
Last edited:

jpanhalt

Well-Known Member
Most Helpful Member
The footprint (aka package) is pretty much done. Note the unusual numbering pattern. It is numbered looking from the bottom, not top.

Some questions:

1) For the symbol, there are several options with respect to design. Some people put the pins in the same order as on the chip. That cannot be done exactly like that with this chip, because of the central pins. Do you want them grouped by function? (I prefer it that way for MCU's.)

2) The stencil is for applying solder paste. It is, I believe, the t-DOCU layer. I can add it or leave it off. Check with your assembler regarding the thickness, hence pad length to be used.

3) Pin 98 is in the ground-pin cluster; however, it is not supposed to be connected in any way. Do you want me just to leave it off? That will cause a gap in the numbering sequence. In smaller chips, I usually leave the unconnected pins shown and just not connect them. In this case, considering where Pin 98 is located, there may be a risk that it will get electrically connected to ground, which will not work. On the other hand, a ground pour might put copper there and that could be a problem. I would not use a ground pour under this chip, but if I did, I would make sure there was no copper under Pin 98.

4) Check with your assembler about solder mask. Do you want it excluded from around the inner pads? My concern is that a solder mask may raise the chip up enough that the inner pins will not get soldered. I have no experience with this type of chip.

I will begin work on the symbol and will group pins by function until I hear from you.

John
 

jpanhalt

Well-Known Member
Most Helpful Member
Here is a revised zip file with the package and symbol. I have not connected them yet.

Look at the package labeled "copy". I did that in case something got inadvertently moved. Please confirm the pin numbers are correct.

For the symbol, please check whether the direction assignments (e.g,. I/O, PWR) are correct. Also, now is the time to move the pins around, if you think a different arrangement would be easier to use. I though about putting all of the ground pins on a separate part of the symbol (like different gates of a logic device), but found only a few instances of that being done.

John

View attachment 62603
 

Wilksey

Member
Hi John,

Wow, you have done so much! I really don't know how you do it so quickly.

In terms of time frame, I am just grateful that you are helping me, so I can wait if necessary!

In terms of solder paste etc, I will probably have a go at the hand soldering technique used on the Cinterion youtube blog, so the larger pads would be advantageous to me.

Grouping by function will be absolutely fine.

I would say leave pin 98 in, chances are it wont get soldered if it is in the ground cluster for any prototype stuff.

Do you think the pins are far enough apart not to require a solder mask?

I will probably hand solder to begin with as mentioned so I am not too worried about the solder mask, whatever looks correct I guess?

I will not use a copper pour on the top layer, I always put the ground pour on the bottom and use vias if required.

If I do want to get the boards assembled outside in the future i'm guessing that the solder mask can be changed at a later date?

(Bit of background info)
The problem is, all of our PCB work where I work to is done by an outside company, we provide schematics and a BOM and they give us gerbers and a bill, which is fine for commercial stuff as the revenue is recouped, naturally I thought i'd quite like to have a go at PCB design and read several articles and video blogs etc, and was going fine until I came across drawing dimensions and footprints that I had to draw, most of the components I use are either in the eagle library or from adafruit / sparkfun etc, which is fine, they are proven (most are anyway!), so I have no issues there.

So all of my personal projects (non commercial), is literally me + eagle free edition, we use Proteus and Cadstar and Altium Designer in work, but of course I don't have access to the floating license servers from home, so I am desperately trying to learn how to make good PCB's, I figured the best way is to just make some, and so far they have worked without issue, I mean I wouldn't do it as a career full time, but I quite like designing stuff, so what I really want to do is to be able to confidently draw my own SMT components, as I said through hole is not so bad as I can print off the footprint and poke the component through, but LGA is a different matter, so I want to be able to draw them from the datasheet and dimension drawings (and actually know what I am doing!)

I shall check the footprint for direction etc and let you know, i'm sure you have it correct though! I may have to change the pin allocation as they are keeping the footprint but in July there will be a newer version of the BGS2 and it will have a different pin out (typical!).

We use this device commercially at work but I cant port the footprints from the PCB design into Eagle unfortunately!

I think you are 5 or 6 hours behind us time wise.

Again, thank you so much for your help! Do you have any good tutorials that might help me do my own? I've read a lot and just can't grasp it!

Wilksey
 

Wilksey

Member
I just checked the ZIP file, there is only the footprint not the symbol in the package?

Did you have the symbol with the pins?

Thanks,

Wilksey
 

jpanhalt

Well-Known Member
Most Helpful Member
I will attach the file again. You have to extract it, then move the .lbr into the a folder (I just use a single folder). Then use the Eagle dialog to open library. The symbol is BGS2. BTW, would you prefer another name for it?

I just added the stencil with long slots/pads to the package (not included here). After you double check pin numbers, I can assemble and send the completed device. This thing comes without any warrant whatsoever. Have you decided what to do with Pin 98? Right now a pad with NC is being used.

John

View attachment 62612
 

Wilksey

Member
Hi John,

I have done all of the above, in the library viewer it usually shows all footprints and devices inside a library, inside TempETO.lbr it just shows LGA66 and LGA66COPY, no devices, in the schematic editor I "use" the library and nothing shows up in the add dialog for TempETO, if I do the same for the PCB editor it shows the LGA66 and LGA66 footprints.

I even deleted the lbr and copied from the latest ZIP file, still the same, I am using Eagle 6.1.0, I have remote access to my work machine so I tried using Eagle 6.1.0 professional edition to see if that helped but it didn't, I tried on the free edition and it was the same.

Thanks

Wilksey
 

jpanhalt

Well-Known Member
Most Helpful Member
It is not a device yet. It is just a symbol and a package. You need to click on symbol (farthest right icon). Once the symbol and package are linked (there's a pin to net dialog to go through), it is harder to make changes -- at least without first unlinking.

John

Let me know if yo can't find the symbol again. I will write a step-by-step of what I am doing. Maybe there is something obvious we are both missing.

j
 
Last edited:

Wilksey

Member
Ahh, just gone into the library editor and found it in there! Doh! Sorry.

All looks OK apart from RXD1 is labelled RDX1, cant find any fault with it! The footprint looks correct, from a very simplistic point of view anyway!

Thanks

Wilksey
 

jpanhalt

Well-Known Member
Most Helpful Member
OK, I will make that correction. Reversals like that are the bane of my existence. I will use the longer cutouts in the stencil, as that can be changed easily, I think. I will remove the drafting lines, but suggest you keep a copy with them too.

The stencil layer is a yellowish layer in 6.1, I believe. I am still in 5.11, as it made absolutely no difference, except for that color.

John
 

jpanhalt

Well-Known Member
Most Helpful Member
OK, here it is. You have a device BGS2 and the copy in that library. I changed the pin numbers to just #, not P$#, as that is more common.

Let me know if there are any problems.

John

Delete:ATTACH=CONFIG_62617_/ATTACH

Added new: View attachment 62618

Edit: That earlier file may have had an error. This new one checks out fine.

John
 
Last edited:
Status
Not open for further replies.

EE World Online Articles

Loading

 
Top