Test Point Coordinate Extraction / Creating Test Fixtures - Page 1
Forum section: electronics / general

author: Tim51
author_rank: Contributor
timestamp: August 14, 2020, 05:12:42 pm
content: Hi Guys,I currently have a board completely designed in Altium Designer 20 with about +50 test points. I have also created the frame of a test fixture using Solidworks, which I plan on cutting out of 3.55mm (3.55mm is all I have on hand) plastic with a laser CNC. The issue I am having is how to best enter the coordinates for the test points from Altium into Solidworks.My first thought was just take the coordinates from the Test Point Manager from Altium and enter them into Solidworks manually but this is tedious and error prone. So my second thought was export the pcb step file from Altium along with the test point 3d models and then use test points as a reference point in solidworks. I could take the PCB board and make it parallel to the board that would hold the test pogos and then cut holes from the test pogo board that are in alignment with the PCBs test points. But this has prone to be a little more challenging than expectedI'm hoping there is a better way to do this. Do you guys have any clue as to what would be thebestway to input the test points from Altium into some kind of CAD to create a test fixture?Thank you for your time

author: Kean
author_rank: Unknown
timestamp: August 15, 2020, 06:32:00 pm
content: I often use my CNC to make up pogo pin test jigs. From memory the steps I used for this was:1. Set up an OutJob to export the test points in IPC-D-356 format, and in the generation options enable CAMtastic autoload for the IPC output (under advanced)2. When running the OutJob test point generation, the gerber layers will autoload into CAMtastic along with testpoint data as additional layers - one for top (ipc_t) and one for bottom (ipc_b)3. Export from CAMtastic as DXF, selecting whichever layers you want data fromThese instructions (or something like them) was what I used as a starting point - enabling IPC autoload bit was the key to making it "work"http://valhalla.altium.com/Learning-Guides/OG0106%20Test%20Point%20Output%20Options.pdfI actually just tried this, and the ipc_b and ipc_t layers in the created DXF were empty. You may have better luck, or find an option I missed.I may have ended up just using the pad data from one of the other layers for the testpoints, deleting everything I didn't need, then loading the DXF into Fusion 360. I've done this before with exports from Eagle. This DXF clean up can be tedious if there is a lot of extraneous data on the same layer with the test points - but less error prone than typing in coordinates. I use a program called CAMBAM for working with DXF files, and creating quite jobs for my CNC. It can also open Gerber files, although they may need to be renamed to .GBR to be recognised.Hopefully this will help. Or someone else can suggest a better way...

author: Kean
author_rank: Unknown
timestamp: August 15, 2020, 06:46:51 pm
content: Just found this which also suggests exporting as IPC-D-350 netlist format, but doesn't explain how to import into (or reformat this for importing to) a CAD/CAM programhttps://designhelp.fedevel.com/forum/main-forum/altium/8838-exporting-test-pointsYou could look at a third party tool like CAM350 - which can import IPC netlists and export DXF.It seems to be US$500 though. Maybe try the evaluation version, and see if it works for your use.Seehttp://www.downstreamtech.com/cam350-connectivity.php

author: T3sl4co1l
author_rank: Super Contributor
timestamp: August 15, 2020, 07:04:45 pm
content: If you need a more machine-readable format than IPC (which is pretty simple already, if maybe not drop-into-Excel ready?), if nothing else you can query TestpointAssyBottom or whatever in PCB Filter, go to PCB List, select columns from Net to X1 and Y1, then Copy. Paste formatting is tab separated, so it will drop into Excel or whatever, or save as TSV, etc.Could even go further and make drawings in Altium for example, but pasting and locating objects is probably more time consuming than other entry methods (and you still have to import the DXP or STEP or whatever).(I've done the latter, just for reference purposes -- sometimes handy to have a printout while working on a prototype.)Tim

author: Kean
author_rank: Unknown
timestamp: August 15, 2020, 07:12:04 pm
content: Actually, using the filter to select and copy all the test points into a new PCB document may be a quicker way than what I suggested (less clean up of the export). Then using CAMtastic you can export to DXF for import to CAD.You may want to first adjust the test point pad sizes in the PCB to suit your CAD requirements. Also maybe include the PCB outline in the new PCB and DXF so you can properly align when importing.If it was only a handful or two of test points, then I'd go with the manual copy/paste - but for a large number I'd try using an export/import even if there are some extra manual steps involved.

author: Tim51
author_rank: Contributor
timestamp: August 21, 2020, 07:19:58 pm
content: @Kean and @T3sl401l thank you for the support. I was able to export all the X-Y coordinates and the IPC but the core of my issue is how to get that information into Solidworks so I can then add it to the test fixture build. I know this is an EE forum but I was hoping someone has some experience with creating a test fixture in Solidworks.I ran with a solution based off @Kean's first option but with a twist:In Altium remove everything from my PCBA but the test points and the board > Export the file as a STEP > open the PCB step file in my Solidworks test fixture assembly > Mate the top side of my PCB (where all the test points are) to the part of my fixture that will hold the pogo pins, the pogo board > Change the orientation so that its perpendicular to the pogo board > created a new sketch and drew center tapped circles on the pogo board using the test points on the imported PCB as a reference.Its crude and I know there has to be a better way to do this but it wasn't too bad, probably took 20 minutes in all, I can live with that for now.

author: electrolust
author_rank: Unknown
timestamp: August 23, 2020, 02:12:52 pm
content: Quote from: Tim51 on August 14, 2020, 05:12:42 pmExport as DXF.https://www.altium.com/documentation/altium-designer/edaexporter-dlg-pcbexportsetupexport-to-autocad-pcb-adFrom there I assume you know what to do? You can use the DXF to create coincident holes for your test jig.Or, use Solidworks PCB to import gerber.

author: JesusCastane
author_rank: Newbie
timestamp: September 29, 2020, 12:33:23 pm
content: Parasolid allows to include copper features.So maybe you can select the testpoints with "IsAssyTestpoint" and then go export/parasolid/export only selected copper.Maybe that helps!