Add various Samtec mezzanine footprints from the Q Strip/Q Pairs, Basic Blade & Beam, Razor Beam, and mPOWER families #1304
Conversation
|
|
myfreescalewebpage
added
Addition
|
A licensing issue has come up with the 3D models, so a minor revision may be in order. |
|
A footprint pull request is never dependent on contributing a 3d model. All that needs to be done is preparing the footprint to accept a 3d model. (Meaning filling out the 3d model settings such that it is easy to add a model at any time without needing to edit the footprint.) |
|
Why is the courtyard not on a 0.01mm grid? Can you provide that reference? I don't see anything in the drawings linked above. The QTH link above is for the product page. Would http://suddendocs.samtec.com/prints/qth-xxx-xx-x-d-xxx-mkt.pdf (or possibly http://suddendocs.samtec.com/prints/qth-xxx-xx-x-d-xxx-footprint.pdf) be a better link to use? |
Section 2.5 (beginning on p.16) of the HSMC Specification gives exact placement information for the connector and PCB edges. Since KiCad does not support PCB edges in footprints, I placed the edge locations in the courtyard.
I considered using both those links when creating the pull request, but neither of them provides complete information for the exact part I created. The first provides no footprint information, and the second is a generalized footprint for the entire family. If we were to use one of those links, I would probably lean toward the second. |
|
Mark the PCB edge explicit, then. This does not affect the courtyard which should conform to normal KLC requirements. See #570 and several footprints in the library (search for "edge" in the footprint name). This is not in KLC so I understand it's not obvious what to do. In combination don't those two docs cover everything? What is missing when both are included? |
|
I see. Maybe something about PCB edges should be added to the KLC. Since the HSMC specification sets the width of the board, should I put a PCB edge label on three sides? Those documents do cover everything, but the footprint description only allows a one URL. I will revise the HSMC footprints with the PCB edges denoted in Dwgs.User. Do I need to make a new pull request, or is there a way to make the change in this one? Since the physical connector is off-center in the HSMC footprints, I'm assuming that I don't need to move the footprint anchor. Also, since the HSMC card specification is so specific, perhaps it would be better to add only the connector footprints and create a template that fully complies with the HSMC specification. |
|
Should the mounting holes used in the footprint also be added to the footprint library? |
|
What would be the reason for the need to define board edges. If this is a pure connector footprint (Meaning it fits into the connector lib) then there should not be any board edge defined. If this is for including a full module on top (or below) of ones pcb then the board edges of that subsystem do not influence the board edges of your own pcb. The board edges of such a subsystem would then be on the fab layer and the footprint would live in one of the module libraries. The only reason i can think of why there is a need for a pcb edge defined is if there is anything in the way. (This would be the case if this is designed to fit into a specific housing that is part of the system for which we design the interface definition here.) Edit: Ok i think i understand now. This is a quasi standard that defines a maximum for 3 sides of a pcb with 2 or 4 mounting holes and a connector. (The pcb is open to extend in the 4th direction.) The connector footprint alone would still be added to the samtec library. If special mounting holes are needed to create the template then these should be added to the mounting hole library. Also note that the specification is given as looking from above. So the connector would be placed on the bottom in that template for easier review. (As one would need to mirror it in ones head otherwise.) |
|
HSMC is a standard developed by Altera (now Intel FPGA) for expansion cards that attach to FPGA development boards. After realizing that templates exist (I didn't until after developing the footprints), I agree that only the connectors themselves should be placed in the footprint library. Thus, I plan to port the |
|
Please let me know when you've made the changes and are ready for a review then. Thanks! |
…Minor edits to ASP-122952-01 and QTH-090-x-D-A connector footprints.
|
@evanshultz As suggested, I am going to migrate the HSMC_Card footprints to templates, and have thus removed them completely. A few minor edits were also made:
|
|
As long as you have a GitLab account as described in the README, you can just keep working on this PR as before. |
|
@chschlue I do have a GitLab account with the same email as this account, both are public. The reason I've narrowed the scope is so that I can use the GitLab repo instead of this one once it is available. |
…KiCad#2466) The existing footprints have reversed pin ordering, so that pad 1 does not match that on the datasheet or indicated by the pin 1 indicator on the connector itself. The footprints are created with kicad-footprint-generator with ``` smd_single_row_plus_mounting_pad.py conn_molex.yaml ``` Footprints generated by this script must always have pin 1 on the left-most side, so in order to fix the numbering the connectors are rotated by 180 degrees. This update also fixes incorrect tags that specified "top entry" instead of "horizontal". (cherry picked from commit 8750227)
vertical connectors
in Connector_Samtec_QStrip.pretty so that the links work correctly
calebreister
changed the title
|
I've created a new script capable of generating all of the vertical Razor Beam connectors (LSHM, LSS, LSEM). This includes the LSHM connectors, a few of which are already included in the Connector_Samtec library. Shall I delete the old versions of these connectors from this branch since newer versions are now available in Connector_Samtec_RazorBeam? |
|
Razor Beam connectors: Samtec 3D model fit test: |
|
There is one minor instance of clipping: the alignment holes for the LSEM connectors are supposed to be centered at -0.95mm according to the drawing and datasheet, but the alignment pins on the model are closer to -0.1mm. I think that the error is most likely in the model. Even if it isn't, there's enough clearance in the holes and enough space on the pads for the connector to shift 0.05mm. |
calebreister
changed the title
|
Added the Samtec mPOWER connector family (UMPT/UMPS) to Connector_Samtec.pretty. Here are a couple of the new footprints. These are the weld tab variants. They match the Samtec 3D models. |
* Add OnSemi CASE 100AQ, for the QRE1113 sensor This is the Through Hole footprint for the QRE1113 Miniature Reflective Object Sensor, a reflective optocouple Reference: https://www.onsemi.com/pub/Collateral/QRE1113-D.PDF This footprint is required to fix issue 2623 on kicad-symbols KiCad/kicad-symbols#2623 * Add footprint for Everlight ITR1201SR10AR sensor This is the SMD footprint for the Everlight ITR1201SR10AR Miniature Reflective Object Sensor, a reflective optocouple Reference: https://www.everlight.com/file/ProductFile/ITR1201SR10AR-TR.pdf This footprint is required to fix issue 2623 on kicad-symbols KiCad/kicad-symbols#2623 * Fix 3D model file path for Everlight_ITR1201SR10AR and OnSemi_CASE100AQ The fix was in order to make them comply with the KiCad Library Convention F9.3 * Fix OnSemi_CASE100AQ Pad 1 shape, setting it as a Rounded Rectangle The change was made in compliance with the KiCad Library Convention F7.3 * Fix OnSemi_CASE100AQ positioning, setting the origin on Pad 1 The change was made in compliance with the KiCad Library Convention F7.2 (cherry picked from commit 78041bd)
* Use unique and IPC package sizes for R, L, and C (cherry picked from commit 0008170)
(cherry picked from commit 806e461)
|
Since I now have a script that generates all of the Samtec Razor Beam (LSHM/LSS/LSEM) footprints, I have deleted the old LSHM footprints in Connector_Samtec.pretty. |
|
@calebreister Anyway, let's try to get this done. My thought is to review the script and then spot-check some footprints. If that looks good, we pull the trigger on the whole lot of them. If you're willing to handle any script updates if there are problems, so far as you can see (we can't know the future), that should be fine. Let me start with a couple things:
|
Not intentional in the slightest. I tried to merge in changes from each release tag (the most recent being 5.1.7), but may have screwed it up. I'm not sure how to fix that.
It's quite a few connectors, with room for expansion later on. Here is the breakdown:
I created these libraries due to the number of variants and the possibility for future expansion. I've already begun work on making the horizontal variants of many of these footprints. This will cause some of the libraries to nearly double in size. I'm also working on creating a library for the Q2 family of connectors. That will most likely need to be another PR in the (possibly not-so-near) future. I will be happy to oblige with script updates. I've put a lot of work into these scripts and the associated JSON files containing the footprint specifications. I also matched a sizeable sample of the footprints up to 3D models from the Samtec website. |
|
Note that the current script PR has some incomplete/work-in-progress scripts (such as QStrip_Vertical.py) that I haven't touched in awhile. Since I've done some major restructuring, I will likely end up deleting those files and rewriting them in a new branch. |
|
Quick question about the Q Strip/Q Pairs connectors. What should the ground plane pads be called? The planes are independent per bank, but all of the pads within a bank are connected. Currently, they are prefixed with a "P" (for plane) and the bank number (see above). I thought about naming them SH, but they are not technically shielding. |
|
@evanshultz What do I need to do to resolve those conflicts? Can I just delete the files and merge in the upstream master branch? |
This pull request contains footprints for Altera HSMC cards. There are two variations, which use different connectors:
The following footprints were added...
Samtec_HSMC_ASP-122952-01_P0.5mm_Vertical
Samtec_QTH-090-01-x-D-A_P0.5mm_Vertical
Samtec_HSMC_Card_QTH-090-01-x-D-A_3.076x0.932in_P0.5mm_Vertical
KLC Notes:
HSMC_Cardfootprint anchors are centered on the connector, not the courtyard. Changing this would cause issues with the 3D models.HSMC_Cardcourtyards do not align to a 0.01mm grid, since the specifications were provided by the HSMC specification.See also:
HSMC_CardsymbolsThanks for creating a pull request to contribute to the KiCad libraries! To speed up integration of your PR, please check the following items: