500 Card Edge in KiCad?

Help Support GroupDIY:

imloggedin

Well-known member
Joined
Dec 17, 2005
Messages
261
Location
mid-usa
Anyone know how I can get the correct board size and card edge for a 500 series module to start with in KiCad? Thanks.
 

Brian Roth

Well-known member
Joined
Aug 20, 2005
Messages
1,903
Location
Salina Kansas
And to muddy the waters.......more TMI drawings.
 

Attachments

  • 306-015-520-102 - EDAC Card Edge Connector-1.pdf
    110.1 KB · Views: 47
  • Speck 500 ASC-V Mechanical.pdf
    22.2 KB · Views: 50

Brian Roth

Well-known member
Joined
Aug 20, 2005
Messages
1,903
Location
Salina Kansas
One other thing crossed my mind. Back in Ye Olde Days (1970's) , I designed a few boards which required edge connectors. Hard gold plating on the fingers was a standard requirement to ensure longevity of the fingers through multiple insertions/removals of the card.

I was doing the card designs at 2X size using a mylar sheet with a translucent grid sheet under the mylar for placements, both stacked/taped onto a light table, and I used an Xacto knife and a variety of "stickies" sold by Bishop Graphics.

I now distinctly recall a Bishop "sticky" for edge connectors that had a "plating bar". It added a small trace that extended from the tip of each edge finger out to a trace that ran at a right angle along the width of all the fingers. The PCB fab shop required (?) that in order to do hard gold plating of the fingers. After plating, the PCB shop cut/milled off the excess with the plating bar.

I have no idea what fabrication requirements are in this century. A brief websearch found this:


The pic shows the "pip" from the tip of each finger, and the text mentions "plating bar".

Bri
 

mihi_fuchs

Active member
Joined
Sep 21, 2019
Messages
35
Location
Austria / Europe
Hi,

Maybe far too late, but I tried to design some API500 gear and if you or anybody is interested you could use the edges in the attachment (KICAD project). For mounting the front panel I simply used these mounting screw holes (therefore you find the strange holes in the PCB): %product-title% kaufen
UNADJUSTEDNONRAW_thumb_29.jpgUNADJUSTEDNONRAW_thumb_2a.jpg
Worked quite nicely and everything fitted very well. I also attached a pic of the finished build and the PCB itself so you can get an idea.

Maybe it can be of use for you or someone in this forum. Feel free to use it, as long as it is for non-commercial use :) ...

Cheers
Michael
 

Attachments

  • API500_board.zip
    180.9 KB · Views: 39

MidnightArrakis

Well-known member
Joined
Sep 25, 2015
Messages
131
Hi,

Maybe far too late, but I tried to design some API500 gear and if you or anybody is interested you could use the edges in the attachment (KICAD project). For mounting the front panel I simply used these mounting screw holes (therefore you find the strange holes in the PCB): %product-title% kaufen
View attachment 84529View attachment 84530
Worked quite nicely and everything fitted very well. I also attached a pic of the finished build and the PCB itself so you can get an idea.

Maybe it can be of use for you or someone in this forum. Feel free to use it, as long as it is for non-commercial use :) ...

Cheers
Michael
Michael: GOOD JOB!!! on the KiCAD PCB layout!!! But.....

Now.....Keep in mind that I am only a "beginner" in performing PCB layouts, as I have been designing PCBs for over 40-years, starting with "manual hand-taping" methods as Brian as mentioned using the "Bishop Graphics" materials and using a variety of CAD-programs over the decades at all of the different companies I have worked with within the aerospace/avionics, defense, medical electronics, NASA, R&D laboratories, telecommunications and video electronics industries. So, you can take my comments with "a grain of salt", if you wish, OK???

First off.....while "Copper Pours" are generally a good thing, you don't generally want to have them go out to the edge of the PCB for a variety of reasons. It would be preferable to back-off the "Copper Pour" somewhere in the neighborhood of 50-to-100 mils as a clearance. The same would go for your TOP and BOTTOM soldermasks. Secondly.....when you have a "Copper Pour" on both sides of the PCB as you have done, it helps tremendously to connect each of the "Copper Pours" together using what are called "Stitching Vias". What are "Stitching Vias"? "Stitching Vias" are independent "free-form" vias that are typically connected to the "GROUND" net and are placed by the - dozens - all over the PCB. While the "Plated-Thru Holes" of the capacitors and other components that are connected to "GROUND" will connect both of the "Copper Pours" together, "the more the merrier" principle applies here. Meaning, if you consider the via "hole" as a resistor, then the more resistors that you have connected in parallel, the lower the overall resistance will be and that's a "good thing"!!!

Now, this may not be as an important a parameter in an audio PCB, but it - does - become a critical parameter in all of the "RF" PCBs I have designed. Most of my "RF" PCBs end up having several hundred "Stitching Vias" and on the larger "RF" PCBs I have done, the number can reach into the low thousands!!!

Another item you need to keep a watch out for when doing a "Copper Pour" is inadvertently creating what is called an "Isolated Copper Pour". What that is is a "Copper Pour" area that is -- NOT -- connected to anything and is just a piece of "isolated copper" on the PCB. Usually, the use of "Stitching Vias" can eliminate any "Isolated Copper Pour" areas, but they can also be eliminated by how your "Copper Pour" parameters are setup (i.e., line-weight, spacings, etc.). You may have to dig down into the KiCAD setup parameters to see what may or may not be available to change in this regard.

If you would like to send me your KiCAD PCB file, along with its "Project" file and whatever else it takes for me to load-in your PCB design, I could give your layout a better review and then give you some better pointers on PCB layout for your next project. Another member of this forum recently sent me his GERBER files of an API 2520 module so I could modify and update his GERBER data to be more correct. As it turned out, as I was also reviewing his N/C Drill file, I saw some additional errors within that file and I went ahead and corrected those errors for him. After I had e-mailed his newly-generated GERBER and N/C Drill data files back to him, he placed an order with his PCB shop for 100 PCBs and he recently wrote to me to say that his new boards look GREAT!!! He then mailed me 6 of his new PCBs, which I should receive sometime later on today. (NOTE: I also have a special GERBER and N/C Drill data editing program).

I'm just trying to help out!!!

/
 

MidnightArrakis

Well-known member
Joined
Sep 25, 2015
Messages
131
One other thing crossed my mind. Back in Ye Olde Days (1970's) , I designed a few boards which required edge connectors. Hard gold plating on the fingers was a standard requirement to ensure longevity of the fingers through multiple insertions/removals of the card.

I was doing the card designs at 2X size using a mylar sheet with a translucent grid sheet under the mylar for placements, both stacked/taped onto a light table, and I used an Xacto knife and a variety of "stickies" sold by Bishop Graphics.

I now distinctly recall a Bishop "sticky" for edge connectors that had a "plating bar". It added a small trace that extended from the tip of each edge finger out to a trace that ran at a right angle along the width of all the fingers. The PCB fab shop required (?) that in order to do hard gold plating of the fingers. After plating, the PCB shop cut/milled off the excess with the plating bar.

I have no idea what fabrication requirements are in this century. A brief websearch found this:


The pic shows the "pip" from the tip of each finger, and the text mentions "plating bar".

Bri
Brian: Good to hear your story of early PCB designs. Believe it or not.....I -- STILL HAVE -- my "Bishop Graphics" 3-ring binder of PCB "sticky" items and templates. Can you imagine THIS??? >>> I once had to design a 12-layer PCB using the "Bishop Graphics" materials where the PCBs were to be used on U.S. fighter jets!!! If you can remember, there used to be "D-sized" Mylar sheets that had a row of "Alignment Holes" punched along the top-side of the sheet. You used to have this really long metal bar taped down on your drafting table or "light table" that had short "Alignment Posts" on them that were used to align and hold all of your Mylar sheets in one place. I always could never make up my mind if I wanted to use a "Pad Master" sheet or go ahead and put pads down on every layer. Unlike doing PCB designs today, you - REALLY HAD TO THINK - about what you were doing before you did it, or you could kill yourself easily!!!

Then, do you remember the "Good Ol' Red & Blue" days of hand-taping PCBs??? That was certainly a "mixed blessing" when designing a "Double-Sided" PCB back then!!! I think I still might have a couple of my "Red & Blue" layouts rolled up downstairs in the basement somewhere. MAN!!! Those were the days!!!

/
 

Brian Roth

Well-known member
Joined
Aug 20, 2005
Messages
1,903
Location
Salina Kansas
Back In Ye Olde Daze <g>, laying out a PCB was a huge headache. I would spend hours doodling on a legal pad to work out the routing before breaking out the Xacto and Bishop stickies. Compared to this day and age my PCBs were quite simple...almost all single sided. A few I home etched in the kitchen, but typically I sent the "litho film" to local fab shops because they offered solder plating on the traces.

I had found a local guy with a HUGE "stat camera" who would take my hand taped layouts and produce 1/2 size positive or negatives onto litho film. I always had to specify "emulsion up or down" depending on the vendor making the boards.

My boards were typically small in size, but that huge stat camera came into play when I needed things such as litho film for a rack mount front panel to expose graphics onto a silk screen frame in real size. The stat camera had to handle 38"+ "originals" at 2x to make a litho at 19" wide. I also taught myself how to expose the silk screen photo emulsion with the litho layout and did my own silk screening, until finally farming it out to a screen printing house that understood printing durable ink onto a metal panel.

I never messed with the Bishop red/blue concept. The few double sided boards I did were done as two layers of Mylar film stacked atop each other. In the 70's, I avoided double sided/plated through boards like the plague, because the price went up 5x or 10x.....maybe more.

In closing, when I moved my Universe 7 years ago, I still had a cardboard box with Bishop stickies. They were in smallish plastic trays that I bought from a local supplier decades earlier. Out of curiosity I checked those trays, and all of the stickum had failed. I could take a sheet of, say, donuts and shake the backing sheet. The donuts fell off! Trashcan time.

Kicad for me the past several years as I make small boards for a specific purpose, such as this:


The PCB color gives a hint of who fabs those cards. lol

Bri
 

MidnightArrakis

Well-known member
Joined
Sep 25, 2015
Messages
131
Anyone know how I can get the correct board size and card edge for a 500 series module to start with in KiCad? Thanks.
Here's some 500-Series information that you should find to be of some interest!!!

In addition, I am also available to assist you with any of your mechanical and/or PCB designs for your projects. Examples of some of my equipment designs are attached for your review.

/
 

Attachments

  • API -- VPR-500 Series Module Specifications.pdf
    83.8 KB · Views: 34
  • Radial Engineering -- 500-Series Module Mechanical & PCB Specifications.pdf
    1.4 MB · Views: 35
  • JBW-Designed - RACK STUFF -- Assemblies-Chassis-Enclosures-Panels-Systems.pdf
    6.2 MB · Views: 26
  • JBW-Designed -- 2D & 3D Mechanical Detail Drawings - Cables-Foam-Sheet-Metal.pdf
    3.1 MB · Views: 21

john12ax7

Well-known member
Joined
Oct 14, 2010
Messages
1,950
Location
California, US
The fab house will figure things out. You can just make rectangular pads with a note that edge fingers need hard gold plating. Most (all?) will understand what this means.

You probably want to specify gold thickness though (and perhaps nickel too). The default / cheapest option can sometimes be really thin, which reduces the durability / number of insertions.

Prepare for some sticker shock in how much the cost goes up with gold plating.
 

mihi_fuchs

Active member
Joined
Sep 21, 2019
Messages
35
Location
Austria / Europe
Michael: GOOD JOB!!! on the KiCAD PCB layout!!! But.....

Now.....Keep in mind that I am only a "beginner" in performing PCB layouts, as I have been designing PCBs for over 40-years, starting with "manual hand-taping" methods as Brian as mentioned using the "Bishop Graphics" materials and using a variety of CAD-programs over the decades at all of the different companies I have worked with within the aerospace/avionics, defense, medical electronics, NASA, R&D laboratories, telecommunications and video electronics industries. So, you can take my comments with "a grain of salt", if you wish, OK???

First off.....while "Copper Pours" are generally a good thing, you don't generally want to have them go out to the edge of the PCB for a variety of reasons. It would be preferable to back-off the "Copper Pour" somewhere in the neighborhood of 50-to-100 mils as a clearance. The same would go for your TOP and BOTTOM soldermasks. Secondly.....when you have a "Copper Pour" on both sides of the PCB as you have done, it helps tremendously to connect each of the "Copper Pours" together using what are called "Stitching Vias". What are "Stitching Vias"? "Stitching Vias" are independent "free-form" vias that are typically connected to the "GROUND" net and are placed by the - dozens - all over the PCB. While the "Plated-Thru Holes" of the capacitors and other components that are connected to "GROUND" will connect both of the "Copper Pours" together, "the more the merrier" principle applies here. Meaning, if you consider the via "hole" as a resistor, then the more resistors that you have connected in parallel, the lower the overall resistance will be and that's a "good thing"!!!

Now, this may not be as an important a parameter in an audio PCB, but it - does - become a critical parameter in all of the "RF" PCBs I have designed. Most of my "RF" PCBs end up having several hundred "Stitching Vias" and on the larger "RF" PCBs I have done, the number can reach into the low thousands!!!

Another item you need to keep a watch out for when doing a "Copper Pour" is inadvertently creating what is called an "Isolated Copper Pour". What that is is a "Copper Pour" area that is -- NOT -- connected to anything and is just a piece of "isolated copper" on the PCB. Usually, the use of "Stitching Vias" can eliminate any "Isolated Copper Pour" areas, but they can also be eliminated by how your "Copper Pour" parameters are setup (i.e., line-weight, spacings, etc.). You may have to dig down into the KiCAD setup parameters to see what may or may not be available to change in this regard.

If you would like to send me your KiCAD PCB file, along with its "Project" file and whatever else it takes for me to load-in your PCB design, I could give your layout a better review and then give you some better pointers on PCB layout for your next project. Another member of this forum recently sent me his GERBER files of an API 2520 module so I could modify and update his GERBER data to be more correct. As it turned out, as I was also reviewing his N/C Drill file, I saw some additional errors within that file and I went ahead and corrected those errors for him. After I had e-mailed his newly-generated GERBER and N/C Drill data files back to him, he placed an order with his PCB shop for 100 PCBs and he recently wrote to me to say that his new boards look GREAT!!! He then mailed me 6 of his new PCBs, which I should receive sometime later on today. (NOTE: I also have a special GERBER and N/C Drill data editing program).

I'm just trying to help out!!!

/
Hi,

Wow, I was not expecting something like that reaction - thanks a lot! Yes it was one of my first designs and to be honest, I'm reworking the schematics and the design at the moment as I got audio through the unit, but I had some design flaws in it right away.

I am just starting out in designing PCBs and every note or suggestion is highly acknowledged here, especially from you and the background you just rolled out!

Regarding the copper pours on the design I faced the problem that in another built the two GND-networks interferred with each other. On research in the net I read somewhere that regarding the difference in potential they may act like capacitors in some cases and therefore produce noise in audio circuits. As I removed the second plane the PCB circuit produced far less noise.
Is the reason for additional vias the same then?

I should hopefully be finished with the new design soon, so maybe I can approach you then for a check up and suggestions on the design? That would be great. It's a very well known circuit: 500 series Level-Loc project

Anyways, thanks for the awesome reaction and your time to write the response and your offer. These things are highly acknowledged by a newbie like me :)!!!

Wish you a nice evening,
Cheers
Michael
 

mihi_fuchs

Active member
Joined
Sep 21, 2019
Messages
35
Location
Austria / Europe
Still curious......is a "plating bar" required in the PCB layout for hard gold plating of edge fingers, or can the fabricator figure it out when they see the design?
Hi Brian,

Thanks for your reply and the question. I never ordered it gold plated but as I have now inserted the cards several times for try outs one can already see that the pads are getting worn off. So it would have been a wise decision to read through your previous post before ordering ;-) ...

So definitly one should ask for GOLD PLATING when using the design i posted.

Cheers
Michael
 

mjrippe

Well-known member
Joined
Dec 27, 2011
Messages
2,681
Location
Brooklyn, NY
I have just started to look into designing a 500 series PCB myself, so this thread is a wealth of information! Thank you all. I'm sure I'll be back with questions.
 

JAY X

Well-known member
Joined
Jan 9, 2009
Messages
571
Hi!

I just finished a layout, and i placed some stitching vias in large copper areas. I always build my prototypes with self etching single layer boards, despite being designed as dual layer boards. The drawback is that i don't know the effect of stitching vias until I ask for a board to a pcb manufacturer. In my two layer layouts there is always copper below a signal or power trace.

Attached is a picture of a section of a pcb layout. just to have some opinions about the stitching vias.

Jay x
 

Attachments

  • example of stitching vias.jpg
    example of stitching vias.jpg
    63 KB · Views: 32

MidnightArrakis

Well-known member
Joined
Sep 25, 2015
Messages
131
Hi!

I just finished a layout, and i placed some stitching vias in large copper areas. I always build my prototypes with self etching single layer boards, despite being designed as dual layer boards. The drawback is that i don't know the effect of stitching vias until I ask for a board to a pcb manufacturer. In my two layer layouts there is always copper below a signal or power trace.

Attached is a picture of a section of a pcb layout. just to have some opinions about the stitching vias.

Jay x
[some opinions about the stitching vias] -- In general....."the more the merrier"!!! Just make certain that they are all connected to the -- same -- "GROUND" net, whatever it is that you happen to call it. "Stitching Vias" are the one type of via where the "pad size" and "drill size" can be the "same size", since they are essentially being buried within a "Copper Pour". However, you >> DO NOT << want to cover both sides of a "Stitching Via" with a solder mask!!! If you really do that, as the PCB goes through the wave-soldering process, the air and/or gases within the via hole will expand and blow through the solder mask!!! NOT a good thing to take place. You -- CAN -- cover one side of a "Stitching Via" with a solder mask, just not -- BOTH -- sides!!!

If it is at all possible, I would try to place "Stitching Vias" within the "Copper Pour" areas between your J5 and J102 with a solder mask covering them on the TOP SIDE of your PCB and exposed on the BOTTOM SIDE. This is to ensure that these copper areas are actually tied to "GND", otherwise, they become tiny antennas resonating at God-knows-what frequency. While you can claim that these copper areas -- ARE -- connected to the larger "Copper Pour" by the thin slits of copper that is between the connector pads, you also need to realize/understand that those "slits of copper" will probably more than likely be dissolved as the entire PCB goes through its etching process. If so, then the end result will leave you with "floating unconnected copper" in between all of the tracks between those two connectors. You can either, A) Place a "Copper Keepout" there in order to prevent that area from being flooded, or B) Place "Stitching Vias" within those copper areas and slightly alter your track routing with "jogs" in order to accommodate these vias. Your call.....

In today's world.....there is nothing to gain from trying to design a "single-sided" PCB because nearly and practically -- ALL -- PCB laminate material these days are made as "double-sided" material. If you design a "single-sided" PCB these days, the PCB fabricator will actually use a "double-sided" laminate and simply just etch off all of the copper from one side!!! So, what's to gain??? "In the old days".....-- YES!!! -- "double-sided" PCB laminate material WAS more expensive. But, now.....with hardly - ANY - "single-sided" boards being designed and fabricated anymore, it just isn't financially economical for the laminate manufacturer to create a product that is rarely called for or used anymore. Therefore, the PCB fabricator stocks up on the standard "double-sided" laminate material and just etches off one side of a PCB panel whenever a "single-sided" PCB is required. All of that perfectly good copper is just washed down the drain only because you didn't want to use it. What all of this boils down to is.....just stick to designing "double-sided" PCB's and you will be "Good To Go"!!!

This concludes today's class on "Stitching Vias" and "Copper Pours"!!! You may now return to your regularly scheduled daily activities!!!

/
 

Bo Deadly

Well-known member
Joined
Dec 22, 2015
Messages
2,726
Location
New Jersey, USA
Hi!

I just finished a layout, and i placed some stitching vias in large copper areas. I always build my prototypes with self etching single layer boards, despite being designed as dual layer boards. The drawback is that i don't know the effect of stitching vias until I ask for a board to a pcb manufacturer. In my two layer layouts there is always copper below a signal or power trace.

Attached is a picture of a section of a pcb layout. just to have some opinions about the stitching vias.
I'm not sure I understand. What's the question? Are you saying you want to request a single layer board from a two layer design? I don't see how that would even be accepted.

Otherwise, stitching together ground planes should be fine. But usually it's only done for thermal reasons. With enough vias it turns that area of the board into a decent heat sink.
 

JAY X

Well-known member
Joined
Jan 9, 2009
Messages
571
Hi!,

No. I did the prototype pcb etching it myself on a one layer board. But the final production unit will be two layers, with the bottom layer as ground plane.

I just wanted to make sure that stitching vias as the picture is ok.
Yes, there are some layouts with higher density vias that act as thermal pads. But this is not my goal.

As for your answer, I think I'm in the right track. Thank you very much!

Jay x
 
Top