PCB Fooprint for Samtec Connector

Groover · November 20, 2017, 9:04am

Hello, I am looking for PCB footprint dimension information for the SMT Samtec FTSH 0.05" headers. In general I like to draw my own footprints as I have been burned in the past with libraries.

Samtec don’t seem to provide any drawings, which is irritating. They do provide some files for other PCB packages:

https://www.samtec.com/products/ftsh

I really don’t want to have to download, install and learn Eagle just to be able to open the file and read out out the measurements.

Does anyone have any pointers for me? Note that this is for an ARM-Cortex 10-pin debug header.

Thanks!

Rene_Poschl · November 20, 2017, 10:02am

Kicad can open eagle footprints.
(Unless you run a recent nightly build. There the eagle import seems to be broken.)

1.21Gigawatts · November 20, 2017, 10:18am

The drawing is on the website at the link you provided. Scroll down to the section “3D Models” and click on the “2D View” tab.

Groover · November 20, 2017, 10:24am

Thanks. The Samtec website gives me a LBR file. I tried loaded that into the footprint editor - didn’t like it.

For the 2D view all I see is through-hole mechanical drawings, nothing relating to SMT.

1.21Gigawatts · November 20, 2017, 10:34am

http://suddendocs.samtec.com/prints/ftsh-1xx-xx-xxx-dv-xxx-xxx-mkt.pdf

http://suddendocs.samtec.com/catalog_english/ftsh_smt.pdf

Groover · November 20, 2017, 10:39am

Thanks - but I don’t see the PCB footprint on those documents, only mechanical drawings I.e. I would like to use the manufacturers recommendations for pad sizes, etc. Am I overlooking it?

1.21Gigawatts · November 20, 2017, 10:44am

http://suddendocs.samtec.com/prints/ftsh-1xx-xx-xxx-dv-xxx-footprint.pdf

Groover · November 20, 2017, 10:50am

Perfect!!! Many thanks!

1.21Gigawatts · November 20, 2017, 11:04am

Sorry, in your first post I read “dimension information” and “Samtec don’t seem to provide any drawings”, but I missed the “footprint” part. Although creating footprints from mechanical drawings is fairly trivial, all three of these documents were found from the link you provided.

Groover · November 20, 2017, 11:52am

No problem - I really appreciate the help. I see where you found the PDF on that page now!

erichVK5 · November 20, 2017, 12:23pm

The following utility is able to convert Eagle libraries into discrete gEDA PCB footprints (.fp), which Kicad can load. This might save you some reinventing of the wheel.

I just tested it on

~/Source/translate2geda$ java translate2geda FTSH-105-01-XXX-DV-K.lbr
Using filename: FTSH-105-01-XXX-DV-K.lbr
FTSH-105-01-XXX-DV-K.fp
FTSH-105-01-XXX-DV-K_FTSH-105-01-XXX-DV-K.sym

and it seemed to behave nicely.

Regards,

Erich.

Rene_Poschl · November 20, 2017, 12:31pm

Again. Kicad should be able to import eagle libs directly. No need to go the route via an external script and the gEda format. (Yes i know it is currently broken in nightly but still… If nobody uses the direct import of eagle libs the bugs will never be found and ironed out.)

@Groover could you tell me what kicad version you are using and how you tried to open the eagle files?

I tested it in my older nightly version (which behaves the same as kicad stable)

Groover · November 20, 2017, 1:05pm

I was trying to import it as a single footprint not a library. However I just tried it again. KiCad 4.0.7.

Footprint editor
Preferences -> Footprint Libraries Wizard
Files on my Computer, Next
Choose FTSH-105-XX-XX-D.lbr, Next

Dialog shows “INVALID” for status, format = Eagle, Next

To Global Library Configuration, Finish

Nothing seems to happen.

Rene_Poschl · November 20, 2017, 1:08pm

I will test it later today on my 4.0.6.

Groover · November 20, 2017, 1:09pm

Update: FTSH-105-01-XXX-DV-K.lbr works for me.

Rene_Poschl · November 20, 2017, 1:12pm

Ok FTSH-105-XX-XX-D is in the older binary format. (pre eagle 6)
I fear this has never been supported. (Strange that samtec has a mixture of different file format versions.)

@erichVK5 can your tool handle the old eagle binary format?

erichVK5 · November 20, 2017, 4:54pm

We have just finished off some code for Eagle Binary (v3, v4, v5) layout loading in pcb-rnd, which can save layouts in Kicad format for any Kicad users needing to convert Eagle binary layouts, but we have not looked at binary format Eagle libraries yet.

In case it may be of help, this is what I have been able to extract with some diagnostic tools as far as packages go from the binary format FTSH-105-XX-XX-D library:

(Layer 51 is tDocu, the documentation layer (can mostly be ignored), and Layer 21 is front silk)

  - Package FTSH-105-XX-XX-D: limits (-147mil, -159mil), (150mil, 158mil), desc 0.050"X0.050" CL THROUGH HOLE TERMINAL STRIP ASSEMBLY, 10PINS., subsecs 22
    - Pad: at (-0.100000", -0.025000"), diameter 0.040000", drill 0.028000", angle 0.000000, shape round, first 0, stop 1, thermals 1, name 1
    - Pad: at (-0.100000", 0.025000"), diameter 0.040000", drill 0.028000", angle 0.000000, shape round, first 0, stop 1, thermals 1, name 2
    - Pad: at (-0.050000", -0.025000"), diameter 0.040000", drill 0.028000", angle 0.000000, shape round, first 0, stop 1, thermals 1, name 3
    - Pad: at (-0.050000", 0.025000"), diameter 0.040000", drill 0.028000", angle 0.000000, shape round, first 0, stop 1, thermals 1, name 4
    - Pad: at (0.000000", -0.025000"), diameter 0.040000", drill 0.028000", angle 0.000000, shape round, first 0, stop 1, thermals 1, name 5
    - Pad: at (0.000000", 0.025000"), diameter 0.040000", drill 0.028000", angle 0.000000, shape round, first 0, stop 1, thermals 1, name 6
    - Pad: at (0.050000", -0.025000"), diameter 0.040000", drill 0.028000", angle 0.000000, shape round, first 0, stop 1, thermals 1, name 7
    - Pad: at (0.050000", 0.025000"), diameter 0.040000", drill 0.028000", angle 0.000000, shape round, first 0, stop 1, thermals 1, name 8
    - Pad: at (0.100000", -0.025000"), diameter 0.040000", drill 0.028000", angle 0.000000, shape round, first 0, stop 1, thermals 1, name 9
    - Pad: at (0.100000", 0.025000"), diameter 0.040000", drill 0.028000", angle 0.000000, shape round, first 0, stop 1, thermals 1, name 10
    - Line: from (-0.125000", 0.067500") to (0.125000", 0.067500"), width 0.005000", layer 51, style continuous
    - Line: from (0.125000", 0.067500") to (0.125000", -0.067500"), width 0.005000", layer 51, style continuous
    - Line: from (0.125000", -0.067500") to (-0.125000", -0.067500"), width 0.005000", layer 51, style continuous
    - Line: from (-0.125000", -0.067500") to (-0.125000", 0.067500"), width 0.005000", layer 51, style continuous
    - Line: from (-0.145000", 0.087500") to (0.145000", 0.087500"), width 0.005000", layer 21, style continuous
    - Line: from (0.145000", 0.087500") to (0.145000", -0.087500"), width 0.005000", layer 21, style continuous
    - Line: from (0.145000", -0.087500") to (-0.145000", -0.087500"), width 0.005000", layer 21, style continuous
    - Line: from (-0.145000", -0.087500") to (-0.145000", 0.087500"), width 0.005000", layer 21, style continuous

It looks like a pretty simple array of pins with an enclosing silkscreen rectangle. It should also be noted that pad sizes, and dimensions including drills and diameters usually need to be doubled from the encoded binary values, and this seems to be the case here.

So, in answer to your question, no, the translate2geda utility can’t do binary format.

erichVK5 · November 27, 2017, 1:21pm

A bit more code, and we now have the ability to import binary format eagle libraries as well as Eagle binary format layouts into pcb-rnd.

Here’s is the FTSH-105-XX-XX-D footprint discussed above rendered in pcb-rnd:

This is an important milestone, because the resulting layouts can be saved in Kicad format, and loaded in pcbnew:

This means that community contributed and commercially supplied footprints in the older Eagle binary format are now accessible to FOSS tools such as gEDAPCB, pcb-rnd, and Kicad.

The new code is currently in svn head but should be in the upcoming release (with further refinements) for those who need to convert any binary libraries or layouts.

Libraries containing more than one part produce a layout with all parts centred on (0,0) but these can be dispersed in the layout editor.

Regards,

Erich.

Bretrand · November 19, 2019, 6:10am

It seems now we can have the mechanical drawings or 3D models on TraceParts, with also the footprints and symbol. I didn’t find for all part numbers but you can see everything for free before to download. Well, seems everything is free by the way. Here is an example: https://www.traceparts.com/en/product/samtec-200-mm-low-profile-terminal-strip-tmm-116-02-f-d?CatalogPath=SAMTEC%3AF_SAMTEC001001002&Product=10-20092018-109295&PartNumber=TMM-116-02-F-D