I am working on a design, where I need various smaller printed ciruit boards (PCBs), e.g. a dozen sub-pcb for a dozen seperate LED/Footswitches, one sub-pcb for the input buffer mounted directly on the input jack, a relay-pcb and so on. I usually use ITADs prototyping service for PCBs but never had this requirement. Now I found this:
http://support.iteadstudio.com/support/solutions/articles/1000160585-pcb-panelization-rules
With a total of approximately 20 small PCBs for one build (it's a looper pedal with a lot of switches, relays etc.), I obviously need exactly what they describe as not possible or more pricey (in the context of prototyping PCBs)
Questions:
- Does anybody have experience with them? Are they really charging extra for a couple of slots in my PCBs?
- I would actually like to stay with ITEAD, as I know that they make working PCBs from my files. Nevertheless: Any recommendations for another PCB-fabbing-service, that is not so picky?
- Technical: I've seen some devices, where the boards chip off really nice (e.g. the Cascadia overdrive). Any hints on a good combination of drill hole diameters, distance and PCB thinckness is welcome.
Elecrow will do vScore panels at no extra charge if it is all the same design. If you have more than one board on a single panel there is an up-charge but it's not very much. If it's all the same PCB design then the only requirement is that the panel is 80mm sq. minimum.
For example, here is the panel for my 3PDT boards below. The dimension layer has the overall board outline (100mmx100mm) then each individual board has a dimension outline. The green lines are the vScores. When I output the Gerbers, I include the vScore layer I created in Eagle in the GML file. Then I simply create a new text file that says "vScore on GML layer" and include that in the zip with all the Gerbers. That's all there is to it.
Very cool. I will test their service soon! Thanks!
OK, I tried to panelize, however, I want the components to be labelled identically on each (sub-)PCB. The only tutorial I found was this one: http://diy.viktak.com/2013/02/tutorial-panelizing-pcbs-in-eagle.html
Is that the way to go?
Yes. Run the panelize.ulp, then create a new board where you copy that board with the panelized names in there as you wish, select the proper layer in the CAM job.
Quote from: madbean on November 14, 2018, 09:20:12 AM
Elecrow will do vScore panels at no extra charge if it is all the same design. If you have more than one board on a single panel there is an up-charge but it's not very much. If it's all the same PCB design then the only requirement is that the panel is 80mm sq. minimum.
For example, here is the panel for my 3PDT boards below. The dimension layer has the overall board outline (100mmx100mm) then each individual board has a dimension outline. The green lines are the vScores. When I output the Gerbers, I include the vScore layer I created in Eagle in the GML file. Then I simply create a new text file that says "vScore on GML layer" and include that in the zip with all the Gerbers. That's all there is to it.
OK, it's been some time, but as I am getting closer to ordering, here are my remaining questions:
- Which line width do you choose for the v-scores (I guess 0.0)
- Is there a minimum distance between the sub-PCB-dimension and the v-score?
- How do you receive your boards (e.g. in your example) - one big PCB that you have to crack apart? How do you get rid of the rectangular cutouts on each sub-PCB (top left and right) or the 45 degree angle (bottom left and right)?
Thanks,
Matthias
Forget my questions from above, this image answers all my questions:
(https://www.multi-circuit-boards.eu/fileadmin/_processed_/1/c/csm_leiterplatte_ritzen_macro_0a43b2de25.jpg)
Also interesting: Just found this on https://www.muffwiggler.com/forum/viewtopic.php?t=157892&sid=fdb4e9c2499c7cad7b7685964336c420
(https://www.muffwiggler.com/forum/userpix2/10917_img_0454_2.jpg)
Quote"For my protos in Eagle I arrange several boards in one .brd file (you have to copy/paste with the schematic closed - and be aware that parts references will change if things have the same names). Space boards by 0.05", keeping their out-lines intact. Then draw 0.05" routing paths between and add snap-holes in suitable places. My regular proto place typical charges an extra $20 or so on top of proto price for this."
Not really useful for my current project, as elecrow would charge much less than that for an additional PCB... but still... fantastic, what people come up with!
Quote from: Marshall Arts on February 02, 2019, 10:45:57 AM
Quote from: madbean on November 14, 2018, 09:20:12 AM
Elecrow will do vScore panels at no extra charge if it is all the same design. If you have more than one board on a single panel there is an up-charge but it's not very much. If it's all the same PCB design then the only requirement is that the panel is 80mm sq. minimum.
For example, here is the panel for my 3PDT boards below. The dimension layer has the overall board outline (100mmx100mm) then each individual board has a dimension outline. The green lines are the vScores. When I output the Gerbers, I include the vScore layer I created in Eagle in the GML file. Then I simply create a new text file that says "vScore on GML layer" and include that in the zip with all the Gerbers. That's all there is to it.
OK, it's been some time, but as I am getting closer to ordering, here are my remaining questions:
- Which line width do you choose for the v-scores (I guess 0.0)
- Is there a minimum distance between the sub-PCB-dimension and the v-score?
- How do you receive your boards (e.g. in your example) - one big PCB that you have to crack apart? How do you get rid of the rectangular cutouts on each sub-PCB (top left and right) or the 45 degree angle (bottom left and right)?
Thanks,
Matthias
I'm not Brian, but I panelize boards in Eagle, so I'll take a crack at it:
1.) Yep, 0 line width. It may not matter, but that's what I use. The important thing is to put it on the dimensional layer.
2.) I can't remember the absolute minimum distance. I generally use 3mm, but I think it may be 2.54mm. The other option is zero space between boards. The edge is defined on two boards with a single cut. I don't do it this way, but it can be (and maybe I should).
3.) They show up panelized and I break them free myself. They are generally good enough to use as is (if anything, the Chinese fab houses make the v-cut too deep). If I'm feeling picky, I just file the edges flat. It only takes a few strokes with a fine toothed file.
The red panel in the pic you posted is not v-scored, it uses mouse bites. That's more like what Osh Park uses. That requires a bit more clean-up but gives a sharper edge where it's routed. I prefer v-score for pedal PCBs, but there's no real wrong answer.
V-Lines on the the dimension layer? Brian includes the vScore layer I created in Eagle in the GML file and adds a textfile that he did it this way... I guess it doesnt matter too much.
I found another surprising info for me in this instruction:
https://www.elecrow.com/wiki/index.php?title=How_to_export_gerber_files_from_eagle_file
They say, I should display all layers before starting their custom cam-process, which I have never done with my previous PCB provider (ITEAD). I usually just leave the defaults (with the exception for the vScore layer, of course). Does the settings have an impact on the Gerber output at all?
Just checking, before I send off an order for 50 bucks... Input welcome!
I recently did V-cuts with elecrow (the mini-bypass that you'll get soon). I just added the lines in layer 46 (milling) and a comment with my order that I wanted to use that layer for v-scoring. I also added the .brd just to be safe.
you can download a CAM job for eagle from elecrow that will give you the files you need to order. I only had my usual layers (dimension, top bottom copper, name, stop, etc.) + milling displayed.
My pcbs were rectangular pieces. I'm also interested in how Brians pcb are separated with the irregular shape. Also, I did only had the dimension layer in the circumference of the panel, but not in between single pcbs.
Overall it was easy with my design. I manually renamed the parts since there were so few of them. Elecrow did however alter the array from 2x2 single pcbs to 5x4. I guess they did to fully fill one fr4 piece. In the end I've got approximately 120 instead of 40 boards :D
Quote from: Marshall Arts on February 05, 2019, 07:05:33 PM
V-Lines on the the dimension layer? Brian includes the vScore layer I created in Eagle in the GML file and adds a textfile that he did it this way... I guess it doesnt matter too much.
I found another surprising info for me in this instruction:
https://www.elecrow.com/wiki/index.php?title=How_to_export_gerber_files_from_eagle_file
They say, I should display all layers before starting their custom cam-process, which I have never done with my previous PCB provider (ITEAD). I usually just leave the defaults (with the exception for the vScore layer, of course). Does the settings have an impact on the Gerber output at all?
Just checking, before I send off an order for 50 bucks... Input welcome!
The only issue I've had with panelization in Eagle is when I ran the panel ULP and didn't change the CAM file to use the secondary silkscreen layer (it's tnames and bnames - 125, I think). The primary tnames and bnames will not allow you to use the same name more than once, so all my parts were incremented for each board. The boards worked, but the silkscreen was a mess. So now I have a separate CAM job for panels that works fine.
As far as v-scoring, I would follow the order with an email to the customer service and explain what you want and have them verify that your files will work. Both Elecrow and iTead are usually pretty good about helping make sure it's right.
Quote from: pickdropper on February 06, 2019, 12:47:11 AM
Quote from: Marshall Arts on February 05, 2019, 07:05:33 PM
V-Lines on the the dimension layer? Brian includes the vScore layer I created in Eagle in the GML file and adds a textfile that he did it this way... I guess it doesnt matter too much.
I found another surprising info for me in this instruction:
https://www.elecrow.com/wiki/index.php?title=How_to_export_gerber_files_from_eagle_file
They say, I should display all layers before starting their custom cam-process, which I have never done with my previous PCB provider (ITEAD). I usually just leave the defaults (with the exception for the vScore layer, of course). Does the settings have an impact on the Gerber output at all?
Just checking, before I send off an order for 50 bucks... Input welcome!
The only issue I've had with panelization in Eagle is when I ran the panel ULP and didn't change the CAM file to use the secondary silkscreen layer (it's tnames and bnames - 125, I think). The primary tnames and bnames will not allow you to use the same name more than once, so all my parts were incremented for each board. The boards worked, but the silkscreen was a mess. So now I have a separate CAM job for panels that works fine.
As far as v-scoring, I would follow the order with an email to the customer service and explain what you want and have them verify that your files will work. Both Elecrow and iTead are usually pretty good about helping make sure it's right.
I might be mistaken but I think the panelise ULP generates new silkscreen layers with the correct info on them, this is in addition to the original silkscreen layers
You just have to make sure that when you run the CAM processor that you select the new silkscreen layers for your panelised board and not the existing ones for output to the gerber file.
I have two CAM files saved. One for "normal" pcbs, and one for panelised pcbs, they are identical except for the silkscreen layer output.
Quote from: PMowdes2 on February 06, 2019, 09:37:30 AM
Quote from: pickdropper on February 06, 2019, 12:47:11 AM
Quote from: Marshall Arts on February 05, 2019, 07:05:33 PM
V-Lines on the the dimension layer? Brian includes the vScore layer I created in Eagle in the GML file and adds a textfile that he did it this way... I guess it doesnt matter too much.
I found another surprising info for me in this instruction:
https://www.elecrow.com/wiki/index.php?title=How_to_export_gerber_files_from_eagle_file
They say, I should display all layers before starting their custom cam-process, which I have never done with my previous PCB provider (ITEAD). I usually just leave the defaults (with the exception for the vScore layer, of course). Does the settings have an impact on the Gerber output at all?
Just checking, before I send off an order for 50 bucks... Input welcome!
The only issue I've had with panelization in Eagle is when I ran the panel ULP and didn't change the CAM file to use the secondary silkscreen layer (it's tnames and bnames - 125, I think). The primary tnames and bnames will not allow you to use the same name more than once, so all my parts were incremented for each board. The boards worked, but the silkscreen was a mess. So now I have a separate CAM job for panels that works fine.
As far as v-scoring, I would follow the order with an email to the customer service and explain what you want and have them verify that your files will work. Both Elecrow and iTead are usually pretty good about helping make sure it's right.
I might be mistaken but I think the panelise ULP generates new silkscreen layers with the correct info on them, this is in addition to the original silkscreen layers
You just have to make sure that when you run the CAM processor that you select the new silkscreen layers for your panelised board and not the existing ones for output to the gerber file.
I have two CAM files saved. One for "normal" pcbs, and one for panelised pcbs, they are identical except for the silkscreen layer output.
Yep, that's the exact scenario I tried to explain and the exact solution I ended up with.
My mistake the first time was using the original CAM file that used the original tnames/bnames. Since then, no issues.
I was trying to help prevent him from walking the same path I did. :-)
Thanks, guys. Guess I can order now... Well their holidays end February 13th :-)
I've found on Eagle 9, the cam file that elecrow provides is treated as a 'legacy' format. It still works, but eagle won't let you select different layers when using it.
You can open the cam files in a text editor, find the list of layers you want to change, and resave the file, that worked for me when I wanted to do panel stuff and had different silkscreen layers.
Eagle 9 also puts up a big scary message about incompatible legacy stuff when using the elecrow cam file - the manufacturing still worked fine for me even with the warning. It was complaining about the drill layer alignment I think.