linistepper v3 single side board (step motor driver)

[sphinx]

hi.
i have made a single side pcb of the project linistepper version 3 from these sites.
http://www.piclist.com/techref/io/stepper/linistep/LiniV3_bld.htm
http://www.romanblack.com/lini.htm
software used is altium version 15.1.15.
i am no expert i just doing it for myself for home projects, i guess improvements can
be done with smd components and other placement i was lucky to only use one via
on the board. i am providing all information except hex file for pic.
have fun with it, if you make changes to the board please share the updated revision.
/mike
password is the usual one

i was a bit to hasty so some changes need to be made to the mounting holes its all.

feedback is allways welcome, i allways appreciate to learn more

update made some minor changes to the board and added smaller mounting holes.
its a work in progress.

(for those that downloaded this if you going to use it check for errors and report
them back, so i can fix it)

[sphinx]

i made more changes and adjustments to the project board size is changed to according
to design size of pcb. modified some components to make make better distance between
tracks. fine tuned tracks, changed mounting holes position and size

/mike

[sphinx]

hi

i made some kinda-sort of bigger adjustments to the pcb design. i compressed the components
around the pic. i modified some pcb layouts so i could fit the components closer to each other
i added another via to make it easier to compress the design easier. there are no changes to
the schematics so thats same so those that downloaded the previous one can still use it.
i modified the resistors R11-13 only to be able to get the "desing rule check" without any errors
the only thing that i changes is the biggish yellow square.

i will leave the other download if you want to use it instead

[sadman]

hi

i made some kinda-sort of bigger adjustments to the pcb design. i compressed the components
around the pic. i modified some pcb layouts so i could fit the components closer to each other
i added another via to make it easier to compress the design easier. there are no changes to
the schematics so thats same so those that downloaded the previous one can still use it.
i modified the resistors R11-13 only to be able to get the "desing rule check" without any errors
the only thing that i changes is the biggish yellow square.

i will leave the other download if you want to use it instead

can you please share pcb design in pdf format

thanking you
sadman

[sphinx]

i have tried to export via altium to pdf but so far i am not able to get a pdf to work, all i am
getting is a pdf with just tracks and nothing else. i will try to figure it out and will post when
i succeed.

/mike

[Parmin]

Maybe just print screen and attach as an image file.

[sphinx]

that would work, but i dont think it will be to scale

[sphinx]

sadman and others
herea are pdf of the pcb in 2 versions non-mirrored and mirrored
at last i was able to make them, only drawback is that the holes
are grey i am not able to figure out on how to change that so far.

please check for errors
/mike

sorrry for the inconvenience but i made a mistake with scaling from what i can figure out
its 2.74 bigger than i should be i saw that some time later while i was fiddling with altium
sorry for that.

i am working on that compressed version with some things and will post it later and from
then that will be the only version i will change, modify or add documents to it.
anyway you have "the source" so you can modify it according to your own ideas and wishes.

/mike

[Ichan]

Hi Sphinx,

May I try to re-layout your board? I am going to test single layer auto routing using Specctra (aka Allegro Pcb Router) with this board.

-ichan

[sphinx]

of course u can thats why put the files on here its kinda sort of open source, you can do whatever you
want with the files, please share your work with us.

/mike

[Ichan]

Good, i will post it soon...

-ichan

[sphinx]

just a thing while you fiddle with it, check for errors i might have done in schematics and/or
the pcb. sometimes  one can get blind sort of and not see the errors made or i might hve missed
something.

i have whiplash problem so my mind is not working as it used to i am on heavy medication and i
have severe sleeping problems which doesnt help, sometimes i have periods i am better sometimes
worse, so things for me the schedule is a quite a bit slower compared to when i didnt have any
issues with it.

/mike

[Ichan]

Well, I did not check it... 

I did a litle modification to the schematic, the main idea is to separate the motor supply and ground to the rest by adding two resistor on it, it can be a jumper or zero ohm resistor in real. Also i rearange component placement for the purpose of the idea above, resulting out the power transistors located on the middle of the pcb.

The step of using Specctra for single layer routing (see attached .dsn and .do file for reference):

1. Export from altium to specctra .dsn file (altium also generate the .do file with the same name)
2. Open the .dsn file in text editor, change the top layer type as "jumper" and add jumper components in the library section then save
3. Run Specctra (Allegro Pcb Router is the other name)
4. Browse for the .dsn file and .do file
5. The .do file can be the one generated by altium or your own (attched the one i use)
6. Start the router, select product with ADV and DFM option
7. Let Specctra do the job
8. Write the routes .rte file
9. Import it as spectra file from altium

I get lucky Spectra autoroute it to 100% with only 2 jumpers, and the imported .rte file give zero error on altium

Attached the altium project files where the pcb layout is all auto routed by Specctra, no manual retouch yet. Included also the .dsn and .do file i use.

Note that i did not change the pad size, as this is a single layer board the pads mostly should be bigger.

-ichan

[sphinx]

yes i agree with you on the pads i like them bigger on single layer. i also like the holes to be smaller
since in a project like this i would do the pcb myself and also drill it.

your work looks great

one other thing is about the transistors i placed them on the edge to easier to mount on cooling unit.

/mike

i think there is a tiny problem with the connector J2a the output to cables are turned to the transistors
so putting cables the will be a bit tricky
so it needs to be turned 180 degrees

am i wrong please check.

/mike

[Ichan]

That connector is a symmetric shape part, just rotate 180 deg when soldering it.

If really needed it can be done by rotating that J2a on schematic, update the pcb then rotate the part and make some adjustment on pcb layout.

Try the Specctra thing, you will love it - that is my main point.

-ichan

[sphinx]

i got the specctra 2.9.4 but i think i am going to figure out how to install the same you are using.
can you tell me what software you installed to get that pcb router ?

/mike

[Ichan]

What i use actually Allegro Pcb Router which comes from Cadence SPB 16.60.xxx, i do not know exactly the minor version - attached the screen shoot of it's help about window, it is actually Specctra see the license information.

I only select the Allegro PCB Router alone when installing the Cadence SPB package as i currently only use that one.

-ichan

[sphinx]

hi ichan.

i am not that familiar with cadence products, i installed the pcb router, when i start i use your files as an example
i put in the dsn and do file click ok then i get a second window with a lot of options to use, i was wondering what
you select/use when you are doing the routing. i tried a couple and it look very nice but i need to learn a bit about
auto routing.

thanx in advance

sometimes someone needs eyes to see i saw what option you are using in a message about
thanx ichan

[Parmin]

Sorry to pull this off topic sphinx, but I think better ask now rather than forgetting about it later.

Hey Ichan, could you share your spectra definition file?
I have tried spectra but never get good result due to my definition file is not defined well.

[Ichan]

@Sphinx, yes as shown on the about window my favorite choice is the one with 6U, ADV, DFM, and HP option.

@Parmin, on the attached .rar file on post# 12 there is the dsn file Linistepper.dsn and the do file SmartDo.do i use, try and study both files.

-ichan

[sphinx]

i will read your dsn and do files and look in documents and try to figure out on how it works and what thing
means. i tried your do file and i added about jumper in two places now i just need to figure out on how to
tell router about wire sizes. i will search here and google for specctra documents and will look at cadence
as well, if i get some nice things to read i will share them here as well.

thanx ichan and everybody else for for help i sure appreciate that. i am no expert just a novis on routing
so i am happy for help.

/mike

[kreutz]

How to print pdf file in Altium: http://techdocs.altium.com/display/ADOH/Smart+PDF

I am sorry for showing late on this thread, I hope it helps.

[charudatt]

Hello Gurus,
I wanted to know how I could convert Eagle Library files (foot print) to Orcad Layout. Any utility available. I'm looking for a footprint for a PCB mounted Rotary Switch.