led display layout pattern

Making PCB Layouts, Manual routing, Auto-routing, Copper pouring, Updating from Schematic, Manufacturing Output
Post Reply
Message
Author
MarkH
Posts: 8
Joined: 27 Nov 2018, 11:53
Contact:

led display layout pattern

#1 Post by MarkH » 25 Mar 2021, 05:06

Hi All,

I have a layout job that is pretty daunting coming up, let me paint a picture!
754 leds in a radiating circular pattern generated in solidworks see attached pic
Now I do not want to have to place each part manually it will take longer than I have.

I have been looking at exporting XY point data then inputting the component positions,
I thought maybe I can go into the .dip file and change the XY in bulk?

Has anyone had to overcome such a task?
Untitled.png
You do not have the required permissions to view the files attached to this post.

Tomg
Expert
Posts: 1737
Joined: 20 Jun 2015, 14:39

Re: led display layout pattern

#2 Post by Tomg » 25 Mar 2021, 11:17

1) Replace all of the "X"'s with 1mm circles, delete everything else and export the result as a DXF file (e.g. "LED_array.dxf"). I have included a DXF file (units: millimeters) in a zip folder below if you would like to use it. If so, double-check all of the dimensions to make sure I didn't foul up anything.
2) Import the DXF file as a pattern (Pattern Editor main menu: Pattern > Import from DXF...) into one of your custom pattern libraries (DXF units: same as DXF file, Import Mode: Add, Convert to: Top Pads), give the new pattern a name (e.g. "LED_array") and resave the library.
3) In the PCB Layout editor place the new pattern (e.g. "LED_array") into the Design Area.
4) Right-click on the newly-placed "LED array" pattern and choose "Ungroup Component" in the context menu to reveal what has now transformed into a large group of independent pads.
5) Select/highlight the entire group of independent pads, right-click on one of them (pad must be highlighted in green) and choose "Replace Component..." in the context menu to bring up the Replace Component dialog window.
6) In the Replace Component dialog window navigate to and select the desired LED component, set Apply To: Selected Components and click on the [OK] button. A "Confirm" dialog box will pop up asking "Number of pads differs. Do you want to replace?". Click on the [Yes] button. You should now have your LED array.
LED_array.zip
p.s. You can import the DXF file directly into the PCB Layout editor if you wish, but importing into the Pattern Editor instead will allow easy, precise (e.g. coordinate entry of pattern/array center) and multiple placements of the "LED array" pattern on the PCB before ungrouping to convert into LEDs.
You do not have the required permissions to view the files attached to this post.
Tom

MarkH
Posts: 8
Joined: 27 Nov 2018, 11:53
Contact:

Re: led display layout pattern

#3 Post by MarkH » 25 Mar 2021, 13:00

Hi Tomg,

Genius! I will try it out and report back :)

Tomg
Expert
Posts: 1737
Joined: 20 Jun 2015, 14:39

Re: led display layout pattern

#4 Post by Tomg » 25 Mar 2021, 13:41

One side effect that you will run into is the labels will be turned off (easily turned back on) and the RefDes prefix for the LEDs will be "PAD". The RefDes prefix can be changed en-masse using the following procedure (make a PCB file backup copy before starting)...

1) Now that you have an array of LEDs with the incorrect RefDes prefix go to the main menu and select File > Export > DipTrace ASCII..., save the ASCII file to a convenient location such as the desktop, clear/delete all objects in the Design Area and resave the original PCB file.
2) Using your favorite ASCII editor open the newly-created ASCII file, replace all instances of "PAD" (upper case, don't include the quotes or suffix/number) with "D" (upper case, don't include the quotes) or whatever reference designator prefix you prefer for LEDs (use the search-and-replace-all function with the case-sensitive option enabled) and resave the ASCII file.
3) Close the ASCII editor.
4) Back in the PCB Layout editor open what is now the blank original PCB file, in the main menu select File > Import > DipTrace ASCII..., navigate to and select the newly-modified ASCII file and click on the [Open] button. All of your LED reference designators should now have the new prefix.
Tom

MarkH
Posts: 8
Joined: 27 Nov 2018, 11:53
Contact:

Re: led display layout pattern

#5 Post by MarkH » 29 Mar 2021, 04:55

Map VA.png
Hi Tomg,
Thank you for your help. For completeness This worked very well and save me a lot of time and sanity :D
The only gripe I have is there was no way of generating a net list ect but I understand why. So I had route all traces manually it's a shame the Vdd and Vss could not be attached to the pins before importing.
You do not have the required permissions to view the files attached to this post.

Tomg
Expert
Posts: 1737
Joined: 20 Jun 2015, 14:39

Re: led display layout pattern

#6 Post by Tomg » 29 Mar 2021, 12:26

Looks good. Here's something you might want to try on a similar future project in an effort to create a net list and save some time...
1) Drop one LED into a new schematic and connect it to VDD and VSS netports. This will be the first set of objects (wires included). Make sure the connecting wires have the proper net names.
2) Copy and paste the first set. Now you have a group of two "LED/netports/wires" sets.
3) Repeat the process with larger and larger groups of "LED/netports/wires" sets until you have the desired number of component sets.
4) Run the RefDes Renumbering tool and save the schematic.
The above process shouldn't take more than five minutes. Here's a partial view of a typical example...
ra.png
5) Open the PCB LED array file and run the Renew Layout from Schematic tool using its "By RefDes..." option. This will link the PCB components to the schematic components and create all of the necessary nets and ratlines.
6) If you are not worried about transmigration problems between gaps (not intended for outdoor environs), create an all-encompassing VSS ground pour on the Bottom side of the board and a similar VDD pour on the Top side. Update all copper pours. If you are worried about transmigration problems, skip this step.
7) Run the autorouter. It shouldn't take more than five minutes and it might even be entertaining to watch the autorouter come close to choking on all of those components and nets.
8) After the autorouter is finished, update all copper pours again and then rerun the verification checks to clean up any invalid error indicators.
9) Manually clean up any bizarre looking traces that might have been deposited by the autorouter, rerun the verification checks again and resave the PCB file.
You do not have the required permissions to view the files attached to this post.
Tom

Post Reply