carlynorama

the blog

Eagle 30/30 No. 18 – Pretty File Layouts, Boards

by Carlyn Maw on June 19, 2011, no comments

So a quick, last minute, right before midnight post today.  

I needed a way to put indicators on schematics for objects that really only appear on boards.  I’ve created a system with items in rectangles for objects destined for Document Layer (48) and not in rectangles for ones headed to tPlace (21).  Items on tPlace if mirrored will actually be on bPlace.   _BRD shows up in the names symbols and devices that are DOC(umentation) objects that have an effect on the board. Additionally the letters _REF are added to the names for the items on layer 48 – i.e. refereance only, not for printing.

The run down of the new items in the library… sorry no picutres today. They are pretty boring looking anyway even if they’ll save me time.

Symbols
DOC_BRD_REF_AUTH
DOC_BRD_REF_LIC
DOC_BRD_REF_URL
DOC_BRD_REF_FRAME_S

Packages
DOC_FRAME_S
DOC_FRAME_S_TXT (has documentation text on it already)
DOC_REF_AUTHOR
DOC_REF_URL_CRLYNORMA
DOC_REF_LIC_CC3_URL_1-27MM
DOC_URL_CRLYNORMA_1-27MM

Device
DOC_BRD_REF_URL
DOC_BRD_REF_LIC
DOC_BRD_REF_AUTH
DOC_BRD_REF_FRAME_S

 

Eagle 30/30 No. 16 – Intermission: Eagle Environment Configuration with eagleassign.scr

by Carlyn Maw on June 16, 2011, no comments

I’m trying to make my Eagle time more effective so today I’ve spend some time setting up the environment. Required reading?

 

On a side note, the Eagle defaults on a MAC OSX or Linux machine live in a hidden file in your home directory. I think it is what the ASSIGN command changes.  I used BBEdit to look at it. If you are unsure how to see it, open a new terminal window (it usually dumps into the home directory) and type ls -a to see the directory listing of hidden files.  I’ve heard good things about the utility Houdini is command line isn’t your thing and you don’t have a text editing application that can already see them. CadSoft warns against editing the .eaglerc file directly, though, especially while Eagle is open. Fair warning.

 

There will be a little bit more meta tomorrow while I get ready to prep some of the boards for actual production. Whoo hoo!

Eagle 30/30 No. 15 – Sextet of Switches with Hardware Debounce (Day 1 of 2)

by Carlyn Maw on June 15, 2011, no comments

I think I’m going to need two days on these boards to feel final about them.   I’d like to really explain the circuit, pick some better values for the resistors and the capacitors, import the parts into my library, check the spacings on the headers… Unfortunately I can’t get all of that done today.

 

 

The two versions I’m debating is one that can hang off the side of a bread board and one that uses female headers like a Arduino itself.  Right now it’s 4 inches long, it would be interesting to see if i could make it into a shield.  Surface mount parts would take care of that… decisions…

 

 

Tips of the day:
  • Don’t smash parts until really really done. The unsmashed parts give better information about orientation at a glance.
  • Uncross lines in the rats nest (airwires) as much as possible before auto-routing for route path ideas, then rip up the auto-route, flip parts, rinse, repeat. My final route is mostly always by hand, though.

 

Eagle 30/30 No. 7 – NASA Logo and Solder Mount Parts, Via’s, DXF imports

by Carlyn Maw on June 7, 2011, no comments

Okay, so I’m late posting today because I bit off way more than I could chew in the time I had.  Yesterday I got to attend the NASA JPL TweetUp and it was AMAZING! Also since Tod and I had been talking about importing vectors into Eagle I figured I would find an EPS version of the NASA logo and turn it into a board.

This ended up being way more complicated than it need to be, but I learned a lot.  I have a number of screen shots that now make no sense because my process was so iterative and loopy, but here at least is a narrative of how to approach this in the future.

Preping the EPS FILE

The EPS file I found – from NASA btw – was in terrible shape for my purposes. My purposes being following the erudite and insightful tutorial by Tod E. Kurt who really wanted to be able to spend at least some time together in June without watching me draw curves in Eagle… So some of the steps I ended up taking in Illustrator

  • Selecting everything and using the Pathfinder > Divde mode to break things into as many small parts as possible and assembling bigger blocks as appropriate
  • Using the Object > Simplify command with the Object > Path > SImplify tool with the Straight Line Option selected to clean up my paths for import
  • Checked EVERYTHING, TWICE for being really closed if I was going to import it as a polygon, etc because the ULP doesn’t give error messages on DXF import fail, it just fails 
  • Used the Object > Path > Offset Path command to create an expanded shape for the board dimension layer

Things I’d do differently:

  • Switch the units in illustrator the file to mm so I didn’t have to remember my scaling factor on every import
  • Have a registration mark on every layer to help with placement in the eagle import
  • keep in mind that the DXF file records position of the selected object in the file – if I wasn’t  scaling I’d have been able to use that more effectively
  • Made an Offset path for the swoosh’s copper layer.

The Schematic

Each of the small stars is ignored in the schematic. Each of the large stars is 1206 packaged solder-mount LED part from the SparkFun library.  Each set of LED’s gets a current limiting resistor of the same package type. The resistor on the channel with only one LED has a higher Ohm value than the others. When I actually look up the current specs of the LEDs I’ll be able to determine what that value is using Ohms Law (V = IR).

The power source is a 9V batter that can also act as a stand.

Also ALL MY NETS HAVE A PROPER NAME. (used to help bring the vias into play)

The Board

  • First thing I did to layout the board was bring in a tight version of the outline of the logo with the stars cut out of it. This is later deleted.
  • I placed the parts on the board (mirroring the resistors and the battery clip to get them on the back of the board) The LEDs were placed with one pad on the big stars – which I didn’t clean up in illustrator and are now causing all sorts of errors in the board rules, btw.
  • Change the grid to be very very fine after the parts are placed, btw. THis helps with getting the imports registered with each other, etc. (0.1 mm regular, 0.01 mm secondary)
  • I placed Vias at each of the little stars.
  • Lets pretend that I next placed the large swoosh as a polygon on the Top layer (layer 1).  The swoosh comes now because it is on a copper plane and because it is a very good part to use as a registration. COPY THE CODE from the ULP window into a txt editor, we’re going to use it later.
  • And then lets say I did all the traces. Using the name tool to name vias the same as the net that I needed them to connect to.  Helpfully having remembered to draw a little circle on tPalce where all the little stars are in case I needed to rip up mistakes. 
  • Next is placing the cut up version of the NASA on the tPlace layer
  • and then the Orbity thing on the same tPlace layer (these all print as silk screen)
  • And then importing a the Offset outline to the Dimension layer as a wire
  • Adding some accent curves so the logo didn’t swim around in the offset
  • So in the final board the swoosh is a shiny shiny metal, I pasted in the code we so handily copied earlier, with one change – the LAYER in line 4 should be LAYER 29 – tStop. This way the solder mask won’t go there and the tinned copper will shine through. If you do a reimport rather than a copy and paste of the SRC code, remember to make the tStop layer visible first.

I’m sure there is a ton more I could write, but… must… do… other.. things…

Eagle 30/30 No. 6 – One Simple Switch Please and Same Schematic, Same Parts, 5 Boards

by Carlyn Maw on June 6, 2011, no comments

So switches, they’re easy.  Two leads, and a pull up/down resistor depending.    My requirements for this little board is that it be flexible as to what kind of data I’m going to feed a micro-controller (i.e. is

actuated 5V or 0V) and that it make an attempt at making this already ridiculously easy circuit that much faster to plug into a breadboard.

In this version a little tactile momentary button stands in for all switches. You could solder in this button, or solder in wire leads to a different switch.  I don’t like this package design for this purpose, though. I’d like to electrically connect the leads on the board the way they are in the button so the two “extra” holes can be used for a second circuit. Next round.  

Boards A, B and E are 0.5 inches. Boards C and D are 0.6 in.  The longest pcb is 1.5 inches long.

In Version A (left to right, btw) the headers are spaced such that P (for Pull) and I (for Input) can go into the rails of the breadboard, and D for data will reach a row (I measured the distance to be 9/32 inch to the first hole on an older Jameco Value Pro breadboard, we shall see). Since the switch is pretty big, I cut a hole in the board so extra lead lines can be connected to that row.

Version B is the same pin layout but the switch is swiveled off to hang off the side of the breadboard.  A hole for a supportive standoff is at the far edge in case pressing the tact switch starts to lift the pcb out off the breadboard.

Version C has the assumtion that a jumper wire will be soldered into the pcb to connect to the Arduino, and that the standoff is helpful.

Version D, same as C, standoff discarded.

Version E, whole little unit with all the headers all in a row. Can use it across 3 rows, with lead wires, with a lead wire just on the data and headers on the P & I (it’ll eat up bus real estate)….

And the sad thing is – I could easily make 5 more… But not today!  I’ll be at the JPL tweet-up when this posts in the morning and I need some sleep.

Goodnight!

Eagel 30/30 No. 2 – Simple Voltage Regulator & Copying Devices

by Carlyn Maw on June 2, 2011, no comments

Both Adafruit and SparkFun have great little voltage regulator boards. Lots of features, solder mount, fits perfectly across both rails, etc.  I wanted to make a board though, that could be filled with the type of parts that used to be in the supply closet at ITP – through hole, big, what they are changes a bit.

I think I might tune it up better on a subsequent day so I’m not putting up these eagle files for these plans yet, but what I learned so far:

Eagle Command Line = GOOD.

It facilitates things that are impossible to figure out in the UI, like copying parts from one library to another.

For example, lets say you want to build a switch that is sooooort of like another switch, but not exactly like anything you’ve found yet in the library. After making your own new library, with that open you type something along the lines of:

copy devicename.dev@library (.dev/.pac/.sym)
rename oldname newname (renames the one in the open library)

more specifically

copy MS243.dev@switch;
rename MS243.dev sw_2POSTOG;
rename MS243.pac sw_2POSTOG_sm;
rename 320-916.dev sw_3POSTOG;
rename 320-916.pac sw_3POSTOG;
copy creative_commons@sparkfun;

etc.

In a new fresh library, open it – copying that whole block into the command line tool bar will bring you some all of the fresh parts I used to make the switch (which has 5.08mm spacing between the leads. More common is 4.7mm, see the C&K / Mountain Switch and Jameco Value Pro product lines…)

 

 

 

June is Eagle Month

by Carlyn Maw on June 1, 2011, no comments

So I really dislike the circuit board software Eagle… still. This is why I do a lot of my schematics in Illustrator. I like visual control.  Unfortunately visual control doesn’t really help when you’re trying to do cicuit boards – auto generating boards from schematics does. So once again I am going to relearn Eagle by attempting to make 30 boards in 30 days.

Please note there are a couple of alternatives out there, http://fritzing.org/  (with a breadboard view feature) and http://www.upverter.com/ , but they are still a bit raw and Eagle is remains the free standard. There are opensource alternatives – but not so much for the OSX.  OrCAD and Altium (formerly Protel) are two of the big heavies in the schematic capture / electronic design automation field. I, however, can’t quite swing the 5k – and again – not so much with the OSX native.

Fritzing has a great page on the EDA player run down,btw:  http://fritzing.org/about/comparison/

My big references for this adventure: SparkFun tutorials and board designs, various Instructables, vague memories of attempts in the past including Tom Kinyon’s class at CRASH space and harassing Tod, of course.

The first result: Simple TIP120 board for driving a pulsed-pull-type-solenoid. Or a one way motor. As you like.  The reason I emphasize the type of solenoid is that the parts used can stand short bursts of high current, but do not withstand full power for long peroids of time. The amperage can go up to 8 on these babies in the right senario (full volatage, no limiter) so pulsing yes, hold no.

Eagle images attached. I put the file on BatchPCB as CRASH space, although it is single sided and designed to be printable at home.

http://batchpcb.com/index.php/Products/61662

 

Some notes:

  • Part List
    • Connector Terminal Blocks: 2 Position 5.08mm Solder Straight Thru-Hole (At least 15 Amp, 16 to 26 AWG depending on what is hooking up to it, in orig project multiple colors were used)
    • The higher power load, i.e. (12-24 VDC pull type solenoid)
    • High Power Supply (lawn mower batter, etc)
    • Optional Capacitor, at least 100 uF, rated for 100V
    • TIP120 NPN Darlington Power Transistor
    • 1N4004 Diode
    • 1K Ohm 1/4 Watt resistor
    • Microcontroller circuit sold seperately…
  • The terminal block parts are 5.08 spaced terminal blocks from the con-wago-508.lbr,
  • The resistor from rcl.lbr
  • The transistor from transistor-power.lbr
  • Everything else from the latest sparkfun eagle library, including the leads to GND.
  • Capacitor is optional depending on you application and where other caps live in your circuit.
  • If you have commoned your grounds somewhere else in your circuit you only need to run one groundline to the board, either from the micro or the high power source but not both.
  • Min trace width is 0.016 to be friendly to home printing.