• Please review our updated Terms and Rules here

ISA PCB Pattern Layout and Pin Assignment Critique

cr1901

Veteran Member
Joined
Dec 28, 2011
Messages
817
Location
NJ
I happen to use a schematic capture (DipTrace) and PCB tool that comes with an ISA bus edge connector PCB template.

The PCB template, showing the pattern on the PCB, must manually be added to a new generic connector part to be usable within schematic capture (so that when I create a PCB, the connector part I created is associated with the ISA bus pattern). For the purposes of validation, I ensured that each ISA pin is either power, bidirectional, input, or output. Most of these are obvious, but for the purposes of DMA bus mastering (for a potential 16-bit part), I assigned the following pins as bidirectional:
A0-A19, IOR/W, MEMR/W. Did I miss any other pins (besides data) that I should assign as bidirectional?

I was wondering if someone with a pair of precision calipers or a micrometer could tell me whether the following ISA edge pattern is likely to make proper contact with the ISA connector if I were to create a real PCB design using it? The green outline is where one should "cut", but since I want to reduce costs, I'll have the PCB fab cut a rectangle; this is something I would have to do manually (somehow- any suggestions?) after I got my PCB delivered. All units are in inches:
6jEJBC1.png


My gut feeling is that the distance between the bottom of the fingers and the green outline is too long, but each finger's length is fine (as well as the distance between the top of the fingers and the top corner). Additionally, while the distance between the center of each two ISA fingers is correct (0.1"), the fingers themselves seem too skinny (0.04") and the distance between the end of one finger and the start of the next finger is too wide (0.06"). Any thoughts? Would a PCB created this template fit properly into an ISA slot/make good electrical connections to the mainboard?

At least I can modify the already existing part to save time. In fact, the conveniently-added dimensions ARE a modification to the vendor-supplied library :p.
 

Chuck(G)

25k Member
Joined
Jan 11, 2007
Messages
40,260
Location
Pacific Northwest, USA
Yup, your "fingers" are too short--on a random sampling of ISA cards, the depth of the edge connector protrusion is about 0.300" and the fingers extend almost to the very edge--about 0.020" relief between the bottom of the connector and the bottom of the fingers. The fingers themselves are a bit wider (0.050") and longer (0.300" -- they extend right up to the top of the protrusion and a little bit past that)

The Intel 1989 ISA spec is silent on the subject of the connector finger details, merely deferring to the manufacturer's spec. But you can still find it.

That should pretty much answer your question about dimensions.
 
Last edited:

cr1901

Veteran Member
Joined
Dec 28, 2011
Messages
817
Location
NJ
Looks like I'll be making my own part and (probably) submitting it back to DipTrace- an accurate ISA bus pattern is essential :p. Thanks for the numbers- will save me some time touching up my personal copy. One measurement I forgot: I measured the distance between the card edge and the start of finger A31 using a standard ruler for two ISA cards, and it seems to be between 0.06" and 0.07". The supplied template has a width of 0.075", so I bet that'll have to be changed as well.

EDIT: More measurements (same vendor-supplied pattern). The edge length appears correct. The finger width/length and NOT it's center position seems to be the only thing wrong:
7z83MFB.png
 
Last edited:

sergey

Veteran Member
Joined
Jul 15, 2010
Messages
740
Location
Silicon Forest, Oregon, USA
Signal direction:
If you're talking about 8-bit ISA slot (like one on IBM PC/XT), then A0-A19 and IOR/IOW/MEMR/MEMW signals are inputs (to the card). They can be bi-directional in bus master scenario supported by IBM AT and AT clones.

ISA edge connector: In my designs I used 0.07" wide and 0.3" long fingers, with ends of the fingers going all the way to the PCB edge. It worked for me both when ordering PCBs with edges cut straight (e.g. from OSH Park), and when ordering PCBs and specifying 45 degrees chamfer for the edge connector.
 

cr1901

Veteran Member
Joined
Dec 28, 2011
Messages
817
Location
NJ
Page 1-35 of the 1984 IBM 5150 Tech Ref has a diagram of ISA card dimensions, that I seemingly forgot about. It recommends:

  • 0.3" card edge height for the portion placed into an ISA slot
  • 0.6" +/- 0.05 finger (called Gold Tabs in the manual) width
  • 0.1"+/- 0.05 center to center
  • 3.19" card edge length
  • According to the drawing of a sample ISA card, fingers ideally should span the height of the card.
  • According to the same drawing, the 31 fingers on each side should be evenly spaced.

In light of this, I created a composite of IBM's guidelines, ChuckG's and Sergey's observations (don't ask me how 0.3 + 0.018 + 0.007 = 3.1):
TEujKcT.png


Hopefully OSHPark creates some decent boards using this; sergey, I'm assuming based on your chamfer comment that OSHPark permits non-rectangular boards? OSHPark is fine (and cheap!) for a one (three)-off, but I've found the traces to be easily destroyed by soldering iron heat.

... Modifying the EISA pattern, if it's inaccurate, is going to be hell T_T...
 
Last edited:

cr1901

Veteran Member
Joined
Dec 28, 2011
Messages
817
Location
NJ
Sorry, I didn't see that edit... must've been more tired than I thought. Well, that answers any and all questions I (and any other hobbyists looking to make an ISA PCB) should have.

Most PCB layout tools that I've used have an ISA layout (KiCad, Eagle, Altium, and DipTrace at least). I tend to use DipTrace b/c it's the easiest for me to create new parts/modify them. Oh, and getting Gerber Files instead of a .BRD file is nice. :p
 

sergey

Veteran Member
Joined
Jul 15, 2010
Messages
740
Location
Silicon Forest, Oregon, USA
Hopefully OSHPark creates some decent boards using this; sergey, I'm assuming based on your chamfer comment that OSHPark permits non-rectangular boards? OSHPark is fine (and cheap!) for a one (three)-off, but I've found the traces to be easily destroyed by soldering iron heat.

Sorry for late reply...

OSHPark will make non-rectangular boards. They will charge you for the size of the smallest rectangle your board fits in.
chamfer - I was referring to the edge connector on the PCB. Some PCB manufacturers (not OSHPark) will shave the edges at 45 degrees, so that it is easier to insert the card into the slot. In case of OSHPark you can shave/round the edges using a file.

Regarding detaching traces - It usually happens then trace is overheated (too high temperature setting on soldering iron, soldering iron applied for too long). Generally I found OSHPark PCBs' quality to be better than some Chinese made boards, and I didn't have any traces detach yet (I did have that with a Chinese manufacturer).
 

cr1901

Veteran Member
Joined
Dec 28, 2011
Messages
817
Location
NJ
I have provided both the pattern (what goes on the PCB) and the component (what goes in schematic capture) for use in your designs. Have fun.
 

Attachments

  • My_ISA.zip
    4 KB · Views: 7
Top