Author Topic: Problems with downloaded Eagle footprints downloaded  (Read 684 times)

0 Members and 1 Guest are viewing this topic.

Offline Faringdon

  • Super Contributor
  • ***
  • Posts: 1162
  • Country: gb
Problems with downloaded Eagle footprints downloaded
« on: June 02, 2022, 05:46:14 pm »
Hi,
I just downloaded the UCC27533DBVR SOT23-5 gate drive IC footprint from snapEDA (for Eagle).
The footprint has the following problems…

1….The tdocu outline is 2.9mm long for the body length…however, max tolerance body length is 3.05mm
2….Both  tvalues and tnames text is in “proportional” style, instead of “vector”. “Proportional style text should never be used in footprints, since it can change position when file is opened/closed. “Proportional” text is only for presentation type documents, (because it looks neater).
3….The “tplace”  lines are 0.127mm wide……this is too narrow, and may not appear on the silkscreen…it should be 0.3mm
4……Pad edge to pad edge is 3.72mm (wideness). This is a good bit of oversize from the 3mm max on the part….however for hand soldered prototyping, its nice to have more pad oversize than that…..typically at least 0.5mm outward oversize on each pad, so 4mm would have been nicer for hand soldering.
5….The pin 1 marker is laterally outside the pad….instead of more middle…..it therefore may be printed over a pad of an adjacent component. Pin 1 can be marked less protrusively than what they have done…..so not good for very tight boards.
6….The geometric centre of the part is not marked on any layer…..so we have to assume its correct…and if it isn’t then P&P machine will mess up.

Do you know of better footprint download sites for Eagle?

EDIT...sorry ive just seen theres a separate forum here for Eagle
« Last Edit: June 02, 2022, 10:28:19 pm by Faringdon »
 

Offline free_electron

  • Super Contributor
  • ***
  • Posts: 8466
  • Country: us
    • SiliconValleyGarage
Re: Problems with downloaded Eagle footprints downloaded
« Reply #1 on: June 02, 2022, 06:29:08 pm »
rule 1 : stay away from CrapEda (snapeda) , CrapCadsys (samacsys) and all those other footprint services. they are horrible. Their symbols are junk and their footprints often wrong. They can't even locate pin 1 properly on something as simple as a connector
rule 2 : reread rule 1
rule 3 : roll your own
rule 4 : goto rule 1

For eagle i don't know. For altium there are is the altium content vault and the celestial library. Maybe eagle can import those.

general rules L

- silkscreen is generally fine at 0.15mm (6mils) that can be printed by any fab these days.

- pin 1 indicators should be 0.1mm way from soldermask clip to accomodate for bleeding or registration errors. soldermask clip over pad should be 0.075mm

- courtyards should be made to enclose EVERYTHING including silkscreen and pin 1 indicators. that way there awill be no problems with marks overlapping adjacent components

- pin 1 indicators are only needed if a part can be installed wrong. for a SOT25 there is no possibility to mess it up so no pin 1 indicator is required. (there is no such thing as a sot23-5. sot23 = 3 pin , sot 25 = 5 pin sot26 = 6 pin  sot 363 sot 563 and so on... this sot23- thingie started off in the 80's but the official standard has it as sot25 and sot26)

- Pads should be designed for proper heel fillets on gullwing pins. The mechanical strength lies there. The tip on RoHs parts is non wettable anyway.
« Last Edit: June 02, 2022, 06:35:32 pm by free_electron »
Professional Electron Wrangler.
Any comments, or points of view expressed, are my own and not endorsed , induced or compensated by my employer(s).
 
The following users thanked this post: Faringdon

Offline Feynman

  • Regular Contributor
  • *
  • Posts: 166
  • Country: ch
Re: Problems with downloaded Eagle footprints downloaded
« Reply #2 on: June 02, 2022, 08:06:04 pm »
I'm afraid there isn't any source for footprints that satisfies everyone's needs. Footprints from snapEDA and the like are a good starting point at best. And the schematic symbols almost always suck, because it appears to be just an auto-generated box with the pins arranged in numerical order around it most of the time.

I like the approach of pcblibraries.com (third party footprint generator) where you can specify your own set of rules (line widths, silkscreen clearance, pin 1 marking, pin 1 location, body outline nominal or maximum dimensions, ...). You just enter the dimensions of your part and the tool takes all your preferences and pad dimensions for optimal solder fillets into account (based on IPC-7351 and J-STD-001). They have a free of charge version that is limited in functionality. But it should be able to output to EAGLE directly.

Some ECAD tools have similar functionality built in, e. g. Altium and DipTrace. The footprint generator of DipTrace looks very interesting and is available in the freeware. However, I don't know if there is any way to transfer a DipTrace footprint to EAGLE.
« Last Edit: June 02, 2022, 08:10:24 pm by Feynman »
 
The following users thanked this post: Faringdon

Offline Anatrujillo

  • Newbie
  • Posts: 1
  • Country: ve
Re: Problems with downloaded Eagle footprints downloaded
« Reply #3 on: June 07, 2022, 05:18:37 pm »
Hello there!

First, we would like to say that we really appreciate your feedback on the UCC27533DBVR part, at SnapEDA we're a small team of engineers passionate about making free and high-quality CAD models for engineers, and we are always working on improving our processes and standards.

We have reviewed your comments and we would like to hear your opinions about it:

1. For the body length we use nominal values for the body outline of our models since our users have indicated their preference for the nominal basic measurements; also our default is IPC-7351B which requires the nominal body. However, we plan to add other densities soon and we are open to ideas, is there a better approach you suggest?
2. As you mentioned, we currently use the default proportional style, this is because this is the default in Eagle. For this case, our team will definitely evaluate moving into the vector style as per your suggestion.
3. Regarding the "tplace" lines, we try to conform as much as possible to the defaults used by the CAD tool and since most of the native EAGLE libraries use that value, we have also chosen to adopt that in most cases as our default; also, in some cases, we use 0.2mm for certain manufacturers. Could you please share some more insights about why you think it should be 0.3mm instead?
4. We make the calculations for pad sizes and pad location following IPC 7351B. However, we have heard this feedback from others who hand solder their components, so we will consider adding a "hand soldering" pad size option in the future to allow for this, and/or supporting the "Most" density option, which it appears would be more suitable based on your other comments.
5. For the pin 1 location mark, we make sure it doesn't overlap the pad and is near pin 1. However, we can totally see your point for tight boards and we will evaluate establishing a standard for the pin 1 location mark that takes this into consideration.
6. Our geometric center is normally based on the center of the body outline, on the mounting holes if present, or on symmetrical pads. However, we agree that we should add a center mark, we will evaluate adding it to the assembly layer, where do you think would be best to add it?

Finally, for future reference, if you want to report issues you can do so on the part page by clicking on Issues>New issue. We automatically get notified and aim to resolve any issues or questions within 24h. Your opinion is very important because it also allows us to keep improving so we can better serve you all!

Thanks again for taking the time to write this feedback, and feel free to reach out to us if you have any comments based on the above.

Have a great day!

Ana Trujillo from the SnapEDA team.
« Last Edit: June 07, 2022, 06:42:55 pm by Anatrujillo »
 
The following users thanked this post: Faringdon

Offline free_electron

  • Super Contributor
  • ***
  • Posts: 8466
  • Country: us
    • SiliconValleyGarage
Re: Problems with downloaded Eagle footprints downloaded
« Reply #4 on: June 07, 2022, 07:09:38 pm »

3. Regarding the "tplace" lines, we try to conform as much as possible to the defaults used by the CAD tool and since most of the native EAGLE libraries use that value, we have also chosen to adopt that in most cases as our default; also, in some cases, we use 0.2mm for certain manufacturers. Could you please share some more insights about why you think it should be 0.3mm instead?

Make that stuff programmable. in the website you can set line widths and layer usage. when downloading the footprint is generated with correct settings. Store settings in user profile. Things like paste retraction and mask over copper spacing needs to be programmable.
Pads need to be rounded corner for better paste release.

Quote
5. For the pin 1 location mark, we make sure it doesn't overlap the pad and is near pin 1. However, we can totally see your point for tight boards and we will evaluate establishing a standard for the pin 1 location mark that takes this into consideration.
check IPC7351C. dots are gone. they peel off . line adjacent to pin 1 , for BGA or parts where alignment is important : mark the three corners . the corner with pin 1 is NOT marked.
The courtyard needs to enclose ALL elements, including the silkscreen. That way, when doing placement , you can go simply by the courtyards. Since all objects are enclosed there is no risk of objects falling on adjacent components. Courtyard also needs to have the centroid mark

Quote
6. Our geometric center is normally based on the center of the body outline, on the mounting holes if present, or on symmetrical pads. However, we agree that we should add a center mark, we will evaluate adding it to the assembly layer, where do you think would be best to add it?
There needs to be a center mark (centroid)  and it needs to be in the GRAVITY point : the point where the pick and place machine will lift the component. For many parts that is just the center , but on things like right angle connectors and heavy parts that is NOT the case !
That way when you export the pick and place file the coordinates are correct.
Professional Electron Wrangler.
Any comments, or points of view expressed, are my own and not endorsed , induced or compensated by my employer(s).
 
The following users thanked this post: Faringdon

Offline jpanhalt

  • Super Contributor
  • ***
  • Posts: 2340
  • Country: us
Re: Problems with downloaded Eagle footprints downloaded
« Reply #5 on: June 07, 2022, 07:43:28 pm »
Sorry to be late to the party.  I have never used a Snap EDA or UltraLibrarian footprint in Eagle.  Use the Eagle footprint and modify to fit your needs.  Or, draw your own.  Learn to use the tools you have, don't blame them.
 
The following users thanked this post: Faringdon


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf

 



Advertise on the EEVblog Forum