Resistor PCB spacing

[iamnothim]

Hello,

I'm new to electronics but I'm learning a lot.  I'm attempting to recreate a tester for 9 pin dual triode valves.  I've purchased a low end B&K model 606 and ripped it apart.
I am wanting to streamline it down to dual triode valves only.   Beyond the emissions meter, I want to provide provide test taps for my oscilloscope (Rigol DS1052E) and Fluke 88V meter.  To date I've gone through the schematic, and ordered many components.  Some of them are actually correct.

I've got some great docs on Valve technology and many mfg. specifications for the valve types I wish to test.  E188CC, ECC88, PCC88, etc.  I've been able to take the anode/grid curves from the mfg.'s .pdf spec sheet and digitize them thus capturing their coordinates.  My hope is to take sweeps from actual valves and overlay them on top of the manufacturers original specifications, showing how close a valve is to the original spec.  I'm a very long way from there, but I have the 50 year old sweeps digitized.

Being a Mac guy, I'm sitting in the back of the bus for scientific software.  That said I've found a great implementation of LTspice for the Mac.  That is a tremendous help in learning about circuits.  I've also found "Osmond" for laying out a PCB board.  I'm figuring that one out.

My question is pretty elementary.  I've taken calipers and measured the wire diameter, body diameter, and body length, in mm of my resistors and Caps.

When laying out a PCB what is the value of what I'll call the "wire spread"?   The length on adds to the body length for bending the thru-hole leads down?   I need to enter this value into Osmond for each components.  A similar question I have is the wire diameter "fudge factor"?

From my calipers a KOA, carbon film, 68 ohm resistor has a wire diameter of .56mm / 22 mils.  The body is 8.8mm / 346.5 mil
When setting up the component, what value do I enter for hole size and length?  Since I've never made a PCB (but I'm going to) Do you use the same wire/hole size when the component values range from 16 mils to 28 mils?

Lastly,
Is there a way export components from LTspice or to LTspice into or out of Osmond?

Many thanks

[ve7xen]

I've never heard of Osmond, but you might want to check out KiCad (free, open source) or EAGLE ('crippleware'). I believe both are cross-platform and work on OSX, and I think they'll have a much larger following in the community.

I'm lazy, so what I usually do is try to find an existing library for my schematic/pcb editor (I use KiCad) and then verify that it will work with my selected components. For things like resistors this is usually pretty easy. Passive parts are almost always standard sizes and a standard footprint will work fine. If I can't find something, I'll make it myself using the manufacturer's recommended pcb pattern. If they don't provide a pattern, I'd say err on the side of caution and make your holes larger than you think you need them, clearances larger than you need etc.

My equivalent resistor package uses a 10mm hole spacing, 2mm hole diameter, 5mm pad outer diameter.

[iamnothim]

Thank you Very Much !

I didn't think about the mfg's having a pcb pattern.  Gee there's an idea.
I'll look into KiCad since it's working for you.   Hope it supports OSX.

Do the libraries list components by mfg parts or categories?
Do the pad specs for a thru-hole component, in KiCad take into account the spacing required to bend the leads down?
Most of the bodies are 9mm.  Do you bend the leads right at the body?  1 mm sounds tight.
Same question for a Al Cap spread.
So as long as you pads are 5mm you drill center to center with whatever bit matches the wire diameter?  That spec isn't even in the program?

Keep in mind, I've never done this.

[Kremmen]

I've never heard of Osmond, but you might want to check out KiCad (free, open source) or EAGLE ('crippleware'). I believe both are cross-platform and work on OSX, and I think they'll have a much larger following in the community.

Just to be fair, let's not forget Diptrace. Considered superior to Eagle by many, and also available for Mac www.diptrace.com. There is a free 300 pin max edition that should take care of most beginner level circuits.

[ve7xen]

I didn't think about the mfg's having a pcb pattern.  Gee there's an idea.
I'll look into KiCad since it's working for you.   Hope it supports OSX.

I'll warn you now, before you get too deep into it, that the workflow in KiCad is not very...refined. I'm a proponent of open-source software being used for open-source hardware, and I mainly use it for that reason. There's certainly a usability cost versus something like a pirated work copy of Altium. If this is your very first stab at designing a schematic and PCB on the computer you might find it a bit bewildering. The basic workflow in KiCad works like this:

1) Draw your schematic in eeschema. If you need to build custom component libraries you can do that, but these components are just the schematic symbol and pin name/numbers.
2) Export a netlist file.
3) Use cvpcb to match components in the schematic to the footprint they will have on the PCB. e.g. a capacitor is a generic part on the schematic, but you may need to associate each one with a different footprint on the PCB. If you need to create footprint libraries, you can do that too from within the PCB editor.
4) Save the netlist that cvpcb modified
5) Import the netlist into the PCB editor, which loads all the footprints etc.
6) Layout your board by moving the footprints around and drawing tracks on the layers

Most other packages let you move more seamlessly between schematic, PCB, and footprint assignment. Altium does this very neatly in comparison, but I don't know how the other free packages compare.

Do the libraries list components by mfg parts or categories?

It's pretty crude, but you can set it up however you want. Each library file is sort of a section in the component browser. Footprints aren't categorized at all, it's just alphabetic. The included schematic libraries aren't that comprehensive and include mostly standard and 'jellybean' parts. Footprint libraries are basically just standard stuff, you'll need to go hunting (or make your own) for stuff like electrolytic caps and so on. One page that has a good set of basic libraries (schematic and footprint) is here: http://smisioto.no-ip.org/elettronica/kicad/kicad-en.htm

Do the pad specs for a thru-hole component, in KiCad take into account the spacing required to bend the leads down?

Each footprint (in the library) is just made up of a bunch of pads (and other stuff like silkscreen and so on). You can put them wherever you want them, so you need to decide for yourself what spacing is appropriate in the end PCB.

Most of the bodies are 9mm.  Do you bend the leads right at the body?  1 mm sounds tight.

TBH I hardly ever use through-hole parts anymore. SMT is much easier to work with. But that footprint (from the site I linked to above) works fine with the standard 1/4W resistors.

Same question for a Al Cap spread.

These you want to be as exact as possible so the caps will mount flush to the board. Check the datasheet, though again there are standard sizes you can find libraries for.

So as long as you pads are 5mm you drill center to center with whatever bit matches the wire diameter?  That spec isn't even in the program?

If you're fabricating the boards by hand yourself, sure you could do that, just make a 5mm solid pad and drill it 'about right'. If you're having boards fabricated at a PCB house you'll need to choose a drill size and the outer pad size. If that's what you're doing, keep in mind that it's not always clear whether the size you specify is the 'finished' hole diameter (after plating) or the drill diameter (which will be shrunk after plating). Check with your manufacturer or err on the side of caution. Larger holes aren't really a problem, they just waste space on the board. Holes that are too small are a pain in the ass to deal with.

I haven't looked but I bet there are some good threads on here about starting out with PCB design.

[kripton2035]

on this forum people seems quite happy with diptrace
it's not free, but it's not very expensive for private use and has a far better user interface than eagle.
but as eagle was free (until version 5) for small projects, there are a lot of libraries for it, instead of diptrace (for now ?)

[iamnothim]

This is great information guys.
Thanks.

I'm not the greatest with open source apps.  I make mistakes as it is let alone putting together an accurate net list.
Not to mention I'm lazy.

I have no problem paying a moderate price for an application.  Freeware like IRUST.in OS/X implementation of LTspice is brilliant.  No terminal code whatsoever.  Samething for OsmondCocoa PCB for OS/x

I will be sure to look at diptrace and KiCad.
My plan was to begin with DIY etching and drilling.  Make a mess and figure out plan B.
My layout is pretty simple so I'm starting with thru-hole.

Again, I appreciate the direction and I'll save this as notes during my applications hands on.

[ampdoctor]

Software not withstanding, the thumb rule I like to use is 1w resistors get 700thou pad to pad spacing, 1/2w 600, 1/4w 500, etc.  Ideally you want about 100thou between the bend and the body.  This should be approximately IPC standard but I may be wrong so don't quote me on that.  With respect to the pad and hole size, take the nominal lead diameter and add 12thou and round up to the nearest drill size for your hole, then double that value for the pad size.  As far as component to component spacing, I tend to lay out 1/2w and 1w resistors with about 200 thou spacing between them, and 1/4w at around 150 thou.  While you can get them closer, if you've got the board space use it.  This makes getting in and out with an iron a snap if you need to do any rework or repairs. 

If you're unsure about how much room you want or need, just get a section of that el-cheapo perf board from radioshack with 100thou grid, load a few components and see what feels comfortable.  And don't forget to add teardrops to your pads.  Aside from getting a slightly better etch with home rolled boards, it'll reduce the likelihood of inadvertently lifting a pad if you get a bit heavy handed with the soldering iron.

[Codemonkey]

1) Draw your schematic in eeschema. If you need to build custom component libraries you can do that, but these components are just the schematic symbol and pin name/numbers.
2) Export a netlist file.
3) Use cvpcb to match components in the schematic to the footprint they will have on the PCB. e.g. a capacitor is a generic part on the schematic, but you may need to associate each one with a different footprint on the PCB. If you need to create footprint libraries, you can do that too from within the PCB editor.
4) Save the netlist that cvpcb modified
5) Import the netlist into the PCB editor, which loads all the footprints etc.
6) Layout your board by moving the footprints around and drawing tracks on the layers

For what its worth, you don't have to work like this in Kicad. You can specify the footprint names in the components in eeschema (press f with the mouse over a component to edit the footprint field) and not use cvpcb at all.

[ve7xen]

For what its worth, you don't have to work like this in Kicad. You can specify the footprint names in the components in eeschema (press f with the mouse over a component to edit the footprint field) and not use cvpcb at all.

Yeah, I usually find cvpcb is just a bit easier than remembering all the inconsistent package names, but I do use this reasonably often.

The other issue is that the standard schematic symbols almost all show the footprint on the schematic, which is stupid, and it's a pain to manually disable for every device. :|

Thanks for the tip though, and I didn't know about the keyboard shortcut, that will be useful.

[iamnothim]

I went to the KiCad site and from what I read the OSX version isn't quite baked.  Last night I downloaded Diptrace.  I just installed it.  Wow.  runs great on my Mac and looks to have enormous capabilities.

[Kremmen]

I went to the KiCad site and from what I read the OSX version isn't quite baked.  Last night I downloaded Diptrace.  I just installed it.  Wow.  runs great on my Mac and looks to have enormous capabilities.

Good that Diptrace seems to work for you.
I would recommend that you get familiar with the "proper" workflow in order to speed things up and avoid unnecessary work. I use a commercial version of Diptrace for all my PCB work and my workflow is roughly this:

- simulations (outside Diptrace) until the specifics of the circuit or part of it are clear.
- create a schematic
 -- Check that the necessary component symbols are available for the schematic and if not, either find them somewhere of create your own, using Diptrace component editor. I use IEC symbols throughout so almost all component graphics are my own creations.
 -- I always add additional data to newly created components; at least a link to the data sheet and the Digikey and Mouser product codes. Makes ordering a project vastly easier.
 -- In case the component has a standard footprint, there is every chance that it will be found in one of Diptrace footprint libraries. If not, create your own and attach the footprint to the component. You don't need to do this for an existing library component of course, since it will be there already.

-create the PCB from the schematic. If everything is in order, you will get a ratsnest with all component footprints scattered in the PCB editor workspace. If not, Diptrace will complain and you cabn fix now or later.
 -- note that if you cha *** nge any component specifics in the PCB editor, you will lose the changes when updating PCB from schematic, unless you have back annotated the schematic from PCB editor.

There is a huge amount of components and footprints in Diptrace standard libraries. Still, i have found it most practical to create a small number of my own component and footprint libraries and collect / crete the most used components into those. That way you ony need to have a small number of libraries in the toolbar and still have proven configurations of the most used components quickly available.
Another suggestion is to split complex copmponents into multipart symbols in the component editor. That way your schematics won't become needlessly messy as you can have only the relevant part of each component shown in a subcircuit.
Lot of other things but you will get there if Diptrace is the right tool for you.


Edit *** broken sentence...

[iamnothim]

Wow !  Thanks Kremmen.

That was a cut/paste/save as .pdf post.

This is my first electronics circuit.  Ever.  I'm rebuilding an old B&K 606 tester to just test Dual Triode tubes and provide taps to test with a DMM and scope.

It's child's play for most.  It has 6 res, 3 pots, 4 caps, 2 lights, 2 switches, 1 meter, and a 6BN8 valve.  Plus the dual triode under test.

I have only completed adjusting the trans secondary voltage on the 6.3 V heater circuit.  As simple as is gets but a laborious exercise for me. I made several mistakes and almost ordered the wrong resisters.  I was hung up on resister power rating, but a couple of members pointed me in the right direction.  I kept hammering until the parts jibed with their instructions.   Lastly I ran it through LTspice and it all checked.   Small task for others.  I thought I took an EE exam at Cal Tech.

Your advice on parts in DipTrace is very welcome.  I have spent hours on Mouser and Digikey finding a resister matches the power rating, is a current part, and is affordable.  That told me I didn't have the correct parts.  I went back, recalculated and then, guess what, there were many choices for the resisters I needed.

I am a long way from making a board, but I figured I'd set the bar high and go for it. (After 1 YouTube video)
It's an adventure.  I'm going to stick with thru hole for the first one.  I have the shakes too bad to attempt SMD.

Thank you again for taking the time to write the post.  Should anyone care, here is the schematic.

[bingo600]

@ianh

Did you see these (i suppose) but  ...
http://bama.edebris.com/manuals/b&k/606/

/Bingo

[Kremmen]

OK, that should be quite doable. And IMO a "vintage" tube project should be done with thru hole components to stay in the spirit of the thing  . Also finding multiwatt SMD resistors could be a challenge although they do exist.

Since this is a tube project one assumes there will be significant anode voltages. Do pay attention to your track clearances and maybe widths as well. One idea would be to familiarize with the Net Classes in the schematic editor (menu: Objects/Net Classes...). There you can create an arbitrary number of different trace width/clearance definitions and assign them to nets in the schematic. The PCB editor will then honor these and/or warn about violations in the rules check. And do check the rules and connectivity several times during the workflow, because there will _always_ be errors of some kind.

If you feel like it, by all means post your design here after done, if you want comments that is. Others have done so and i think the resulting discussion has mostly been useful.

[iamnothim]

The tester I got on eBay had all the original documents and schematics.
Ran across bama and looked at what they had to offer too.  There are also valve history sites and antique radio forums.
Pretty much everything.  It's so cool.  I found a 200+ page doc on how valves work and their implementation. Filled with diagrams and schematics.

Part of me is learning and part of me is building this as a Heathkit.  Snap, snap, solder, solder.
The whole process is about learning electronics and valves.  I found mfg specs for all the various dual triode valves.  My "vision" is to be able to save scope traces of valves and overlay them on top of the old specs.  Thus seeing is NOS is NOS. rather than some number on a tester.  Below or photos of the my 606 that I will use as a "model"
Thru hole ?   I wonder if it will help.
Do you think it's been had some mods done?

[iamnothim]

@bingo600

Thanks for taking the time to research the 606 manual.  It's appreciated.

I had trouble finding a wooden 3PDP switch from Mouser.
Do you know where I can find one.  Thru hole please.   

[iamnothim]

Hi Kremmen,

I "think" I followed your instructions for DipTrace pad layout and spacing.
I used your recipe in the diagram:
take the nominal lead diameter and add 12thou and round up to the nearest drill size for your hole, then double that value for the pad size.

I used the largest almost the largest resistor lead size of .032.   
I added .012 to the .032 to get .044.  This is a #56 bit.
Next I doubled the hole size to get the Pad size:  .088
DO I use this hole/Pad size for all resistors .032 and down?

 I have one large one that is .035.  I'll treat that as a one off.

The resistor in the diagram is 1/2 W  so I used the .0600 buffer space.  As instructed.
Is there a "buffer" field in the Component Pattern setting?

I also will be using some buss connectors that are .055  Those will be special.
The holes will need to be .055 + .012 = .067  #54 bit.
However the pins are .150 center to center
A .140 Pad size only leaves .01 between the pads.
What do you think the pad size should be in this case.

Many thanks.

[Kremmen]

OK, but are you sure it was I who did the instructing? I suspect it was someone else since i am useless at gauges of any kind, being a metric guy from birth.

[iamnothim]

Oops

[iamnothim]

Hello Ampdoctor?