Help an idiot with EAGLE

[Gary Warner]

Turns out I can save a bundle on the PBC manufacturing if I can send out Gerber files. I've already drawn up the PCB in Pad2Pad's software and it took only 10 minutes.

So I'm trying my hand at Eagle. What a pain. I've got some 'stupid' questions for anyone who uses Eagle.

When I placed the components on the board I ran signal lines connecting this to that. Only the SMD resistor and LEDs got connected in 'auto' mode. Why?

The three switches on the top are 6mm types. I can't get runs to land on the pads centered. Why?

How do I make sure the holes for the switch leads are plated thru and padded on both sides (able to connect by top or bottom layers)?

Where and/or how do I see solder masks?

Once I draw a wire, short of deleting it and starting again, how can I change the line properties (change thickness)?

I've got a gazillion more questions, but for now this will allow me to make some progress.

Sorry to be an idiot here, but this program is driving me nuts. I need to master it because the cost of the PCB's is half what Pad2Pad wants.

Gary
--

[Gary Warner]

Here's an example of how easy Pad2Pad is. Took 10 minutes to re-arange the IC to free up space for printing the buttons. This will save me the printing costs if I just use clear covering.

[joe@tech-mp]

Hi Gary,

Not sure about auto mode since I don't use it.

The grid settings control placement of traces and footprints. There are two settings the primary and the alternate which is activated with the ALT key. Think of these settings as course and fine.

All holes get plated by the MFG process as a given.

The solder masks are layers are 29 top and 30 bottom.

The change command -> width (wrench on menu).

I hope this helps ;)

Joe

[Comatose]

Hi Gary,

Eagle is a pain at first for sure, but it gets better with use.

The first problem i think you're having is a workflow one. You start Eagle in schematic editor, build your whole schematic there, and then switch to the board, which will have all your components and associativity done. Trying to build just in layout is possible, but its a pain in the butt.

Second thing, turn the grid display on. Eagle always snaps to the grid (whatever grid you have defined) which is very useful because it makes it easy to maintain your trace/space exactly. But it also defaults to .05", which is far too large. Turn it down to .01 or .005 and it gets much better. The grid icon is right under the "open file" icon, top left corner.

[Malc C]

As Comatose mentioned, its generally best to produce the schematic and then create the board. There are several tools in the schematic that check for errors such as missed connections (sometimes drawing a wire to a component and it isn't connected, but look it if you follow my drift)

Eagle is a pain to start with, and can be frustrating hunting for the right component in the extensive library files, but once you get used to it its quite powerful and does the job well enough

[westfw]

Your problem with "auto" mode (the auto-router, right?) is probably that
the autorouter grid is set much too large for the components you're using.
(the routing grid is set separately from the placement grid. the reason
your switch don't get connected to is that the pins fall too far from the
default (0.05 inch) routing grid...))

[LukeZ]

I will echo what everyone else has said - working in Eagle certainly is a big pain at first, but with just a few days tweaking you can become a pro. The cost savings associated with the Gerber output is well worth it.

As others have said, start with the schematic editor. Only when you have it down should you create your board.

Also, a very important note: When you do create your board, and you decide you need to make a circuit change, you go back to your SCHEMATIC and make the change. But make sure you have your board open while you make the schematic change, or else it won't get transfered over!!! This can cause a nightmare situation; don't ask me how I know...

The "monkey wrench" button is your friend. That is how you change the width of a trace or any other setting. Alternatively, for traces, you can set up "net classes." Just type in "class" in the command line editor, and up pops the class box (or go to the Edit menu, "Net Classes" is at the very bottom of the list). Then you define a class, give it a name, the width of the trace and spacing and other settings. After that use the "Change" tool (monkey wrench) to assign the class to your desired traces. Later, if you decide to change the settings, you just need to change them once in the class definition, and all your traces with that class will automatically be updated (after you click the rat's nest button).

Learning to use the grid was a Eureka moment for me. As Comatose said, click on the grid icon in the upper left (looks like a bunch of small dots). Set your "alternate" grid to a real small size, then liberally use your "Alt" key while placing or moving items. Also when you are laying down a trace the Ctrl key can come in handy - it will usually force your trace to begin right where your mouse is, rather than wherever the nearest connection is, as Eagle defaults to.

Also when an option is selected, such as the Move option, using the right mouse button will cycle through the various settings within that option. This is real useful as well.

Here's a couple pages with some Eagle tutorials that I personally found helpful -
http://myhome.spu.edu/bolding/EE4211/seniordesign_resources.htm (scroll down a bit)

http://vulcan.ece.ucsb.edu/ece189/tutorials.html

Good luck,


Luke

[LukeZ]

The one thing I can't stand about Eagle though is the asinine way that it zooms in and out with the scroll wheel on the mouse. I have kind of gotten used to it after a while, but it is completely counter-intuitive. They should also really have a "hand" option, kind of like there is in PDF editors, where you click and you can drag the screen around. As it is, to move from one place to another on your screen you usually have to zoom out and then zoom back in on the new place, which is total nonsense.


Luke

[Gary Warner]

Thanks everyone for all the great tips and ideas. Sorry I didn't jump in sooner but I spent the weekend playing golf with the folks in Austin.

I see it's just a bit of a steep learning curve. I'll take all of the advice here and try again

Thanks again.

Gary
--

[Afroman]

"Also when you are laying down a trace the Ctrl key can come in handy - it will usually force your trace to begin right where your mouse is, rather than wherever the nearest connection is, as Eagle defaults to."

I've been using eagle for a year and never knew that! Thanks Luke!

[Gary Warner]

I give up :(

Anyone want to bid this little job for me? I'll pay.

Final Pad2Pad drawing attached.

Gary
--

[westfw]

Looks to me like part of your problem is that the default Eagle package
definitions are more conservative than those in pad2pad. You've got
some FINE traces on that board, and... Have you had one built yet?
In particular, the holes for those switches look on the small side.

How's this look? [Sigh. Other than top and bottom layers being switched!]

[Gary Warner]

Looks to me like part of your problem is that the default Eagle package
definitions are more conservative than those in pad2pad. You've got
some FINE traces on that board, and... Have you had one built yet?
In particular, the holes for those switches look on the small side.

How's this look? [Sigh. Other than top and bottom layers being switched!]

They are .010" - Pad2Pad says it's ok so long as there are no etching-holding points and said I need to keep the runs on the 90 degrees to avoid holding points. The holes on the switch cad files (Omron B3F-1000) shows .0393" (1mm) lead diameter. I set the holes at .065.

That Eagle capture looks great. But I can't use it... see below :o



I really am an IDIOT! It's true. :o

I came back to this thread today to announce this fact, loud and clear. I noticed there's a major flaw in the board. See it?

Hint: It's a PIC12F628

God help me; I'm so stupid :rolleyes:

Gary
--

[Gary Warner]

Fixed in Pad2Pad :rolleyes:

[Gary Warner]

Ok, I wasted all of yesterday trying to do this in Eagle, that's why I wanted to punt. Not one to accept failure for very long, I gave it a go again today. I think I have it done now. Does this look right? How do I define the board size?

Gary
--

Edit: Oops. I see I forgot the signal out run.

[Gary Warner]

Question: Is the layer 30 (bStop) where I should put the masking on the bottom thru-traces? See pix.

I changed it again, locating some cheaper LEDS and resistors in the 0805 size.

Gary
--

[LukeZ]

Gary - looks like you're getting the hang of it.

To do the board outline you just use the wire tool to draw a rectangle where you want the border to be - which it looks like you've done. Then use the Change tool to set it to an appropriate layer. I use 121_tsilk (top silkscreen) but you can also use 51_tdocu and probably some others. I make mine 10 mils wide but again, I think most board houses just look for a line, and don't care exactly how it's composed.

If you see a cross-hatch design over your through-hole pads, then you know that the tob and bottom soldermaks are already applied. That's because the top mask slants one way and the bottom the other. Turn off the tStop layer but leave the bStop on and you'll be able to see more clearly what I mean. So there's nothing you need to do in that regad, I don't think.


Luke

[westfw]

Gary - looks like you're getting the hang of it.

What Luke said...

I would advice using thicker traces where you don't absolutely need them
to be extra fine, and especially on the power traces to the PIC. I like to
put as much ground plane down as I can, both for its current carrying
capability, and so user's clumsy static-laden fingers will tend to get grounded
rather than poking a sensitive input pin. Unless your boards area really
strongly priced so that you need to minimize their size, it might even be
useful to make them bigger, with the switches further from actual components,
for the same reason...
I played with my PCB some more last night, and I came up with something
like this (still upside down...)

[Gary Warner]

Yep. I printed the board out and it's got to be the worlds smallest servo driver ever :eek:. The original proto boards that I etched were 3 times the size and had a materials cost of about $1.50 each, not including my time (especially drilling the 28 holes per board :cool: ).

I'm going to consider increasing the size of the PCB, if for no other reason to make assembly easier. The original goal was to reduce the cost of the PCBs. Still, if the boards go from $0.21 each to $0.45 each that should be doable. And once deciding to go larger, I can go back to leaded parts instead of SMD. I did a quick research last night and I can do this in leaded parts for the same parts cost.

Question: How did you make the ground planes? Is there a built-in function in Eagle to do this or do I have to draw them by hand?

And you are right about thicker runs, especially on the power runs. I've had two of the original drivers fail due to the user shorting the output pins by mistake. Each was easy to fix by opening the covering up and repairing the fused run. Thicker runs might still fuse, but it will be a lot more forgiving for the short term shorting from brushing a metal conductor over the output pins.

Thanks for all the good tips guys.

Gary
--

[LukeZ]

Gary,

To make a ground plane, or any plane, use the Polygon or Rect(angle) tool to draw the shape you want. This can just be a rectangle on the entire bottom of the board. Make sure you selet the top or bottom layer, whichever you want. If you don't select the right layer before you draw the shape, that's ok, just use the Change tool on your rectangle to modify its layer.

Finally, to make it a ground plane, use the Name tool on your shape, and give it the same name as your ground net, or whatever. So if your ground nets are named GND, give this shape the name GND. You may get a message that asks if you want to connect these together, say yes. Then really finally, click the Ratsnest tool and you will see that your shape is now filled in. Where it comes into contact with other GND traces it will connect, and where it approaches other signals it will leave a space. Again it is easy to modify the spacing between the plane and other signals, as well as other settings, by using net classes, as described earlier in this thread.

You can use this same process to create planes for other signals as well, if that were every useful. For example you may want to lay a rectangle of copper for a heatsink or something.

By the way, what fab house are you using, if you don't mind me asking? Are you ordering a large quantity to get those prices?


Luke

[Gary Warner]

Thanks for the explanation Luke.

I'm getting the quotes from EZPCB. They do specify that the traces and clearance is .01". I don't know if that's an absolute or just the minimum, so I don't know just yet if the servo plug runs and ground planes are allowed w/o additional charges. They quote $0.38 for 1000, $0.48 for 500 and $1.04 for 100. This is for the new DIP version on a bit larger board. I'm on the fence right now between the 500 and 1000 quanties.

I sold all of the 25 proto versions in nothing flat and everyone likes them, so I'm going to run at least 500 more. This production run will also have some updated code, involving programing swing limits in the sweep mode.

Like you guys said, it was going to take a few days to get the hang of Eagle - how true. After 4 days now, I can finaly make PCB's w/o pulling my hair out, thanks to your tips.

Gary
--

[LukeZ]

500! Wow, will you be soldering those all yourself? :eek: Or sell them as kits? Using through-hole components and it should be an easy kit for most people to put together.

Well let us know anyways, I might just buy one. ;)

I'm glad you stuck with Eagle and now you're pretty much already an old pro. It's a steep learning curve; frankly I think they made it steeper than it needed to be, but the only alternatives cost big bucks. Learning Ealge has pretty much become a rite of initiation for us poor folks. But now you know it, you can save yourself lots of money and give yourself lots more options when it comes to fab houses.


Luke

[Gary Warner]

Luke,

I haven't considered selling them as a kit. I don't trust most hobbiest to solder correctly (I've seen some very scary stuff at the field). For now, I'll do the assembly. I solder every day so I can do them in my spare time (lots of spare time this time of the year). I can assemble this version all the way down to packaging in 10 minutes or less each. I've got to do something for a living ;).

Gary
--

[Malc C]

Gary,

Sell them ready made. If you sell hem as kits you'll give yourself a headache as customers will be constantly mailing you saying "I've built it and it don't work... can I have my money back or can you fix it ???!"

Sell them as tested and working and you'll be fine ;)

[Gary Warner]

Malc C,

That was the plan. ;)

Gary
--

[Comatose]

Gary, even if you plan to do all the assembly yourself, seriously consider going surface mount. Once you have a solder stencil (which can be as cheap as $30) and some paste ($25) its so much faster to drop chips onto the board then throw them into an oven than solder them all through hole. Of course, a real pick/place and a real reflow oven are ideal, but tweezers and a hacked toaster oven is still much, much faster than through hole.

[Gary Warner]

Gary, even if you plan to do all the assembly yourself, seriously consider going surface mount. Once you have a solder stencil (which can be as cheap as $30) and some paste ($25) its so much faster to drop chips onto the board then throw them into an oven than solder them all through hole. Of course, a real pick/place and a real reflow oven are ideal, but tweezers and a hacked toaster oven is still much, much faster than through hole.

Interesting. Where could I read up on this home-brew process?

The original PCB's were too small to be practicle. So since I had to increase the PCB size, I thought through-hole soldering would be easier because I was going to hand solder the SMD's in place (I do that all the time in my 'real' job, but it does take a fair amount of time). Your idea has me wondering. Once I get a firm quote back from EzPCB I was going to ask about assembly costs (they do that too). It sure would be sweet to open a box, place it and the instructions in a bag and be done.

Gary
--

[cinnamon]

Interesting. Where could I read up on this home-brew process?
--
I found this to be an interesting read: Have you seen my new soldering Iron? (http://www.seattlerobotics.org/encoder/200006/oven_art.htm)

[Gary Warner]

I found this to be an interesting read: Have you seen my new soldering Iron? (http://www.seattlerobotics.org/encoder/200006/oven_art.htm)

Good reading - and shows how to do it without a screen. The cheapest screen I could find was $149.

On another note, I mentioned earlier that I've had a few guys short the pins by accident, damaging the cycler. I found a way tonight to make hoods for the pins for like an extra .02 cents each. Pix show the hooded pins ready to be soldered on the board.

Gary
--

[westfw]

Yep. I printed the board out and it's got to be the worlds smallest servo driver ever :eek:Yeah, it's a bit disorienting to be working on a board for a while on my
lovely large-screen monitor. I lose track of the actual sizes I'm dealing
with, and when I finally print it out it's like Whoa!

[Comatose]

www.pololu.com will laser cut mylar solder stencils for as little as $30. http://www.smtstencil.com/ you just have to ask for the service, they don't advertise it.

[Gary Warner]

Wich of these materials do you use?


We can laser cut:
Note: Plastic thicknesses are nominal and can vary by up to + or -10%.

Acrylic (Plexiglass, Acrylite, Lucite)
1/8" stocked in various colors ($0.05 per sq. in., $4.00 per sq. ft.)
Up to 1/2" also available
ABS (Acrylonitrile Butadiene Styrene)
1/8" stocked in black and white ($0.05 per sq. in., $3.50 per sq. ft.)
Other thicknesses also available
Acetal (Delrin)
Nylon
Styrene
Gatorfoam
Styrofoam
PETG (polyethylene terephthalate glycol)
Woods, cloth, paper, and more!


Gary
--

[Comatose]

Well, for production we get frameless metal stencils for $150 from stencils unlimited, but thats because we run our boards panelized (9-18 up depending on the product), and most of our stencils have four or five different products on them. Stencils unlimited has a fixed price for up to 20 by 20 inches. Also we're running about 1500 units per month at the moment, and plastic stencils wouldn't hold up to that. For proto/low volume work you'd want 4 mil mylar.

[rocky79]

I am new to Eagle PCB too.Does anyone know what layer is used as solder past?
Also When i am creating a new IC package can i draw the IC outline using the wire tool in layer 21tplace?
i have looked at some of the existing libraries and they use a hollow rectangle to draw the outline. I also noticed there is 3 layers on the SMD pads a green(51tDocu) and hatched layer(29tStop). Can anyone explain the common layers used and their functions and some standard pratices.
Thank you

[Malc C]

I'm only a basic user.. still use descrete components rather than SMD :)

Have a look on the Eagle web site as there are loads more library files and you might find that someone has already made the package you want

[Gary Warner]

I am new to Eagle PCB too.Does anyone know what layer is used as solder past?
Also When i am creating a new IC package can i draw the IC outline using the wire tool in layer 21tplace?
i have looked at some of the existing libraries and they use a hollow rectangle to draw the outline. I also noticed there is 3 layers on the SMD pads a green(51tDocu) and hatched layer(29tStop). Can anyone explain the common layers used and their functions and some standard pratices.
Thank you

I think the tStop and bStop can be used, if everything is a pad under the stops. I noted on a solder stencil site, that they can't use the these two layers to make a metal laser cut stencil, though I don't see why not.

This is from the help file on layers:


Predefined EAGLE Layers

Layout

1 Top Tracks, top side
2 Route2 Inner layer (signal or supply)
3 Route3 Inner layer (signal or supply)
4 Route4 Inner layer (signal or supply)
5 Route5 Inner layer (signal or supply)
6 Route6 Inner layer (signal or supply)
7 Route7 Inner layer (signal or supply)
8 Route8 Inner layer (signal or supply)
9 Route9 Inner layer (signal or supply)
10 Route10 Inner layer (signal or supply)
11 Route11 Inner layer (signal or supply)
12 Route12 Inner layer (signal or supply)
13 Route13 Inner layer (signal or supply)
14 Route14 Inner layer (signal or supply)
15 Route15 Inner layer (signal or supply)
16 Bottom Tracks, bottom side
17 Pads Pads (through-hole)
18 Vias Vias (through-hole)
19 Unrouted Airwires (rubberbands)
20 Dimension Board outlines (circles for holes)
21 tPlace Silk screen, top side
22 bPlace Silk screen, bottom side
23 tOrigins Origins, top side
24 bOrigins Origins, bottom side
25 tNames Service print, top side
26 bNames Service print, bottom side
27 tValues Component VALUE, top side
28 bValues Component VALUE, bottom side
29 tStop Solder stop mask, top side
30 bStop Solder stop mask, bottom side
31 tCream Solder cream, top side
32 bCream Solder cream, bottom side
33 tFinish Finish, top side
34 bFinish Finish, bottom side
35 tGlue Glue mask, top side
36 bGlue Glue mask, bottom side
37 tTest Test and adjustment inf., top side
38 bTest Test and adjustment inf. bottom side
39 tKeepout Nogo areas for components, top side
40 bKeepout Nogo areas for components, bottom side
41 tRestrict Nogo areas for tracks, top side
42 bRestrict Nogo areas for tracks, bottom side
43 vRestrict Nogo areas for via-holes
44 Drills Conducting through-holes
45 Holes Non-conducting holes
46 Milling Milling
47 Measures Measures
48 Document General documentation
49 Reference Reference marks
51 tDocu Part documentation, top side
52 bDocu Part documentation, bottom side

Schematic

91 Nets Nets
92 Busses Buses
93 Pins Connection points for component symbols
with additional information
94 Symbols Shapes of component symbols
95 Names Names of component symbols
96 Values Values/component types


Gary
--

[LukeZ]

rocky, I haven't done reflow so I don't know what layer would be used for solder paste. Gary's suggestion sounds like it should work, though wouldn't you still want a distinct stop mask apart from the pads? Perhaps not. This is beyond my experience.

Creating an IC package outline with 21tPlace is fine. If you want to use the outline as part of your silkscreen, I'd recommend you create a seperate layer on 121tSilk. 21tPlace is nice for placement on the screen, but as a silkscreen is usually inappropriate, since for most of the library parts it overlaps pads, which you don't want (this is in spite of the fact that the help file Gary posted lists 21tPlace as the silkscreen - I don't think that can be right). I use 21tPlace for reference within the program, but then create a simplified silkscreen layer using 121tSilk.


Luke

[rocky79]

Guys,
I would like like to ask you, when you made the IC footprint is there any other layers that i need beside those, Also could you check if i am using the correct corresponding layer:
pads : 1top
solder mask: 29 tStop Solder stop mask
solder paste 31 tCream Solder cream
Silkscreen 51 tDocu

Thanks

[Comatose]

A stencil is properly made from Tcream and Bcream. The distincion goes as follows:

Tstop and Bstop are for the cutouts in the soldermask. Board houses require this to be somewhat larger than the underlying pad, because the soldermask film can only be placed so precisely. .003" larger in each direction is common.

Tcream and bcream are the solder stencil layers. These are smaller than the pads, by some amount (.003-.005 is common). This is because the solder paste will squish out the sides somewhat when the componnet is placed on top. If the paste overruns the pad by a significant amount you may get bridging when you reflow it.

[rocky79]

I think i am missing the basics here. let's start from the begining. When i create a part package using smd pads. Does eagle automatically remove the solder mask layer on top of the smd pads and adds solder past to it? or do i need do this manually using the tstop and tcream.
I was just talking with eagle tech support and they said that eagle adds those layers automatically for you. I am now confused...

[LukeZ]

Comatose, I had not known what those cream layers were for, thanks for explaining. That makes perfect sense. When I want to try my hand at reflow now I'll know!

rocky, I think the Eagle people are correct. You don't need to create cream or mask layers when you create an SMT part. They are added automatically. All you need to do is just specify the pad area using Layer 1. Soldermasks and creams are automatically deduced from your pad area using rules you set up. You can modify these rules for each board, you do it in the Design Rule Check (DRC) area. You can open this by going to Tools->DRC or by typing DRC in the command line. Also there is an icon on the left-hand toolbar. When you open the DRC go to the Masks tab for the appropriate settings. You can see the advantage of setting up your masks/cream settings once for the whole board, rather than for each individual part. This allows much greater, and easier, customization.

You might play around with the other tabs in the DRC while you're there. This is actually a very nice aspect of Eagle. For each setting, when you click on it, Eagle displays a visual example of what it is you're modifying, along with a text explanation below it. It really makes it easy to see what you're changing. And, once you make the change, it is automatically applied to your entire board, no work for you.


Luke

[Quacker]

Hi Gary,

If you still need help with Eagle, just let me know. I've been working with Eagle for some years and own a professional copy. I'd be happy to help you--gratis. If you are looking for a solder screen, I can also show you where to get a Mylar screen made for very cheap. Also, it may be better for you to panelize so assembly can be done easily and I can even arrange for my freelance assemblers to crank them out for you.

Best,
Q
(Ira)

[Gary Warner]

Hi Gary,

If you still need help with Eagle, just let me know. I've been working with Eagle for some years and own a professional copy. I'd be happy to help you--gratis. If you are looking for a solder screen, I can also show you where to get a Mylar screen made for very cheap. Also, it may be better for you to panelize so assembly can be done easily and I can even arrange for my freelance assemblers to crank them out for you.

Best,
Q
(Ira)

Wow Q! That's quite an offer. For now (it's been a few days now since I 'gave-up') I've got the files in the hands of the PCB shop and they have checked them and all is well. I decided not to panelize the boards because they charge the same price per square inch, small or large. If I ask for V-cuts, they charge more. If I cut them myself... well, you know... I'll be buying a new band saw blade about every 20 inches of cutting, not to mention my labor.

Assembly should not be a problem. I made a proto PCB this weekend to gauge the assembly time. Parts, 3 minutes, test 1 minute, shrink covering 1 minute, package 1 minute. I figure 6 minutes with a touch of experience, probably much faster as time goes on. I have employees that take extended coffee breaks way too often since we are 'slow right now'. I think I can get some 'free' labor by slave-driving them ;).

For now, this project is going forward with through-hole parts, so it's not going to need screen. BUT, I WILL be needing screens for the Hamster. Oh, that's right... I just remembered... I said I'd let you know as I make progress with the Hamster. I FINALY got Memsic to ship me 10 accelerometers (2.5ms, 400hz output) all be it at retail pricing :( . Now that I have these, the Hamster is scheduled to make a lot of progress in the next month or so. I'm planning on making a proto PCB for these next weekend so I can start fine tuning the code, then it's off to the PCB house for another order. These PCB's will be so small (1x.6") that I'll have to get these on a panel and pay the extra for the v cutting.

Gary
--

[Quacker]

Gary,

My offer stands. I see what you are trying to accomplish and I know how much effort it can take ;o)

Are you able to get boards at .032" thick? If so, cutting will go much easier.

I'm glad to see you finally got some parts. I looked over the Memsic site and asked for a sample to plink around with. We'll see if they ship any.

Ha! I just tried EZPCB on a quote for boards that I will need soon. They matched or slightly beat my last vendor, Gold Phoenix on a 100 pcs of a 5" x 6" board. nice find!

I have a bandsaw and was going to look for a diamond grit blade for FR4. I'm sure that would stand up to the abuse.

[rocky79]

Comatose, I had not known what those cream layers were for, thanks for explaining. That makes perfect sense. When I want to try my hand at reflow now I'll know!

rocky, I think the Eagle people are correct. You don't need to create cream or mask layers when you create an SMT part. They are added automatically. All you need to do is just specify the pad area using Layer 1. Soldermasks and creams are automatically deduced from your pad area using rules you set up. You can modify these rules for each board, you do it in the Design Rule Check (DRC) area. You can open this by going to Tools->DRC or by typing DRC in the command line. Also there is an icon on the left-hand toolbar. When you open the DRC go to the Masks tab for the appropriate settings. You can see the advantage of setting up your masks/cream settings once for the whole board, rather than for each individual part. This allows much greater, and easier, customization.

You might play around with the other tabs in the DRC while you're there. This is actually a very nice aspect of Eagle. For each setting, when you click on it, Eagle displays a visual example of what it is you're modifying, along with a text explanation below it. It really makes it easy to see what you're changing. And, once you make the change, it is automatically applied to your entire board, no work for you.


Luke

Thanks Luke

[Gary Warner]

Gary,

Are you able to get boards at .032" thick? If so, cutting will go much easier.

I'm glad to see you finally got some parts. I looked over the Memsic site and asked for a sample to plink around with. We'll see if they ship any.

Ha! I just tried EZPCB on a quote for boards that I will need soon. They matched or slightly beat my last vendor, Gold Phoenix on a 100 pcs of a 5" x 6" board. nice find!

I have a bandsaw and was going to look for a diamond grit blade for FR4. I'm sure that would stand up to the abuse.

The 1.6mm is the same cost as the .032". It would save a few bucks in shipping and it should be easier to cut.

I tried the sample stuff with Memsic and was told that right now, they were limiting samples to larger targeted manufactures.

EzPCB has been the best price I can find, but I'm sure someone has a better house. The only thing I don't care for with EzPCB is that it takes a full 24hrs to get a email responce. We.ve been batting around emails for a week now and all we've accomplished is a file format correction and payment options. This seems to long now, but with these experiances behind me, my next order should go much faster. BTW, their longest 'lead time' is 10 days DELIVERED. Some of the houses I checked with were upto 14 days before it leaves their house on a slow-boat from China. Still, I'm paying for it - $65 for shipping a ~2 pound box. At least I'm not paying express-fab costs (which can be much higher than express shipping costs).

Gary
--

[Quacker]

Gold Phoenix ran 2 weeks but at least there is a contact in Canada that speaks good English. Everything goes through him.

[Malc C]

not sure what 0.32" equates to in metric, but if it's 0.8mm then you can cut the stuff with a pair of kitchen scissors

[Gary Warner]

not sure what 0.32" equates to in metric, but if it's 0.8mm then you can cut the stuff with a pair of kitchen scissors

Yes, it's .8mm. You don't have probelms with the edges splintering, especialy causing problems if traces are close to the edge?

Gary
--

[Quacker]

I've cut my share of .032" board with scissors but it usually bends it a bit. That makes me nervous if there are SMD parts on it.

[Quacker]

I saw some diamond grit blades for bandsaw out there on the web but haven't priced them. Carbide grit would also do.

[Malc C]

Can't say I've experienced any problems with my boards, although I don't route tracks too near the edge of my boards. I tend to trim my boards before etching anyway

Couple of examples attached

[Gary Warner]

One more question... I promise :p

How do I change the drill size for the micro switches?

The holes are per the data sheet at 1mm, but I'm concerned about the holes being slightly undersized after through-hole plating, or is this already compensated for somewhere?

Edit: I just checked the drill Excellon Drill Station Files and see that the switches will be drilled at .04". The actual leads are .03937". Not much extra clearence, especialy after plating :o . Can I just change the file data for T02 (drills for switches) to a larger standard number?

Gary
--

[Quacker]

Gary,

The best way is to mod the part package in the library. Then return to the PCB and "update" the library. This will change all the placed parts and of course, keep the new hole size for future placements.

Q

[Gary Warner]

Gary,

The best way is to mod the part package in the library. Then return to the PCB and "update" the library. This will change all the placed parts and of course, keep the new hole size for future placements.

Q

ZZZOOOMMM... (hear that?) :eek:

That's you going WAY over my head :D

I've tried to modify and make new parts in the library and never could make it work. Maybe I'll try again ;) .

Gary
--

[Gary Warner]

Ok, here's a good example of how un-friendly this program can be.

Serach help files. Find topic "Editor Windows", click on sub-topic "Library Editor" and it reads:

The Library Editor is used to edit a part library (*.lbr).

After opening a new library editor window, the edit area will be empty and you will have to use the EDIT command to select which package, symbol or device you want to edit or create.


Then I click on ""Edit Library object" and it reads:


In library edit mode you can edit packages, symbols, and devices.

Package: the package definition.

Symbol: the symbol as it appears in the circuit diagram.

Device: definition of the whole component. Contains one or more package variants and one or several symbols (e.g. gates). The symbols can be different from each other.

Click on the Dev, Pac or Sym button to select Device, Packages or Symbols, respectively.

If you want to create a new object, write the name of the new object into the New field. You can also edit an existing object by typing its name into this field. If you omit the extension, an object of the type indicated by the Choose... prompt will be loaded. Otherwise an object of the type indicated by the extension will be loaded.

If your license does not include the Schematic Module, the object type buttons (Dev...) will not appear in the menu.


I've clicked, right clicked and expanded everything in the control panel and NOTHING comes up as Library Editor. I'm sure it's there somewhere, but I can't find it. Would it kill these guys to offer 'help' in the help files?

Back to stumbling around in the dark until I find it :mad:

Gary
--

[Gary Warner]

"Help" was no help :rolleyes: but I did figure it out.

It's File, New, Library. The Open, select "Switch-Omron-lbr". Then Library, Package and slect the package in the list. Then select Change Tool, select Drill and select .043307 as the drill size. Select the pads one at a time, each is enlarged. The save the device, return to the board and goto Library, and select Update All.

Now, was that so hard to explain that the help file can't handle it?

Ignore me - bad mood today :cool:

Gary
--

[Gary Warner]

Ok, another question. I just re-ran the CAM processes and the Drill size is now .0433, and that's .004 clearence. Is that still to close to be reliable?

Gary
--

[Quacker]

I'd say its fine. A .004" over is OK. I believe that board houses generally know that you mean the diameter after plating, and compensate for it.

As for Eagle, the 'help' is useless. The tutorial is better. Best yet is to stop coming at it as if it should act like a Windows program, it doesn't. Your compliant is not so unusual. It does take getting used to but when you get going, it's not so bad.


PS. There aer ways to access the library for editing that is a little faster and less frustrating. (I said a little)

[Gary Warner]

Q,

Thanks for the reassuance about the holes and my dislike of the help files.

I just needed someone to listen to me bitch.

The files are off (for the last time, I hope). This whole PCB house thing is more complicated than I originaly thought it would be. (there I go bitching again :D )

Gary
--

[westfw]

The holes are per the data sheet at 1mm, but I'm concerned about the holes being slightly undersized after through-hole plating, or is this already compensated for somewhere? My understanding is that MOST board houses will use a slightly larger drill to
compensate for the added thickness of the plating. But not ALL PCB houses.
Olimex, for instance, has been dinged in some forums for using a drill that
matches the holesize in the PCB exactly, and then plating and making the
holes just a bit too small...

[Comatose]

Q,

Thanks for the reassuance about the holes and my dislike of the help files.

I just needed someone to listen to me bitch.

The files are off (for the last time, I hope). This whole PCB house thing is more complicated than I originaly thought it would be. (there I go bitching again :D )

Gary
--


Wait til you start having to deal with gerbers...

[Quacker]

Gerber’s are one thing that Eagle makes easy. Unfortunately, they have no viewer included. Fortunately, there are freeware viewers available.

[Gary Warner]

The worst that I had in dealing with CAM files was that EzPCB said "Gerber" files NOT Gerber 274x - that cost me 2 days bouncing back revised files. Then after that was done, I didn't know that Gerber does not include the drill index files. EzPCB was complaining about not having a drill file. So I found out that Excelleon was the CAM process for the drills. There went another 2 days.

FWTW, EzPCB uses CO2 lasers for drilling - must be nice. Is this method of drilling now common place in small PCB orders?

Gary
--

[Gary Warner]

We were talking about solder stencils some posts back. EzPCB sells stainless steel solder stencils for $80 and framed stencils for $130. This is the best price I've seen for these. I think the price is good upto 100 sq. in. but it was unclear as to what the size limits are in my email from them.

Gary
--

[Quacker]

Hi Gary,

Yeah, the Gerber thing can make you crazy. The 274x is appended with drill information unlike the earlier Gerber. My guess is that they have not updated due to $ that might be associated with the laser driver.

I can't answer for other PC houses, but I like the sound of laser cutting since getting slots cut can be very expensive for a hard tooled processes.

If EZPCB uses lasers, they might be my next choice since I have some very large holes in my present commercial board that are only there because of the cost of making a slot.

For your needs, a Mylar screening stencil will likely be your least expensive means. Pololu (mentioned in post #31) is where you get them.

Are you going "lead free?"

Q

[Gary Warner]

Hi Gary,

Yeah, the Gerber thing can make you crazy. The 274x is appended with drill information unlike the earlier Gerber. My guess is that they have not updated due to $ that might be associated with the laser driver.

I can't answer for other PC houses, but I like the sound of laser cutting since getting slots cut can be very expensive for a hard tooled processes.

If EZPCB uses lasers, they might be my next choice since I have some very large holes in my present commercial board that are only there because of the cost of making a slot.

For your needs, a Mylar screening stencil will likely be your least expensive means. Pololu (mentioned in post #31) is where you get them.

Are you going "lead free?"

Q

I think laser cutting the boards is becoming standard practice. I did hear back about V cutting my next order. If I keep the quantity at 500, they will do the V cutting at no extra charge. Since they will be using the seporate my boards from a master sheet as is, it won't make any difference in there investment to make my boards.

I will go Pb free on the SMD projects. I can go either way with the through hole boards. I might make Pb boards ONLY for the California and Europe sales. The last pound of Pb solder I got (SN96.5AG3CU.5) was a steal at $35 because the parts house miss quoted the price. I've been told the next roll will be $69. Hopefully that will be a year or more from now.

Oops, I see on the roll of silver solder that it still has the California warning lable. I guess California considers tin, silver or copper to be cancer causing :rolleyes:.

Gary
--

[Quacker]

I bet it's silver-bearing solder, meaning it's still lead based. True silver solder is very high temp, read torch temperatures.

[Gary Warner]

I bet it's silver-bearing solder, meaning it's still lead based. True silver solder is very high temp, read torch temperatures.

It's labeled "Lead Free Wire" Here's the datasheet (http://www.kester.com/Data%20Sheets/Bar%20Solder/Tin-Silver-Copper%20Global%20(17Feb06).pdf). It has a maximum of .05% (.03% ave.) lead, considered to be lead free (<.1% lead content). I haven't found any solders to have 0.00% lead. Have you?

If I read all of the 'California' label, it may include materials known to cause birth defects or reproductive harm. I guess any heavy metal falls in this category ;) .

I use this to solder STK output IC's in convergence circutit on big screen TVs. Most all the Sanyo STK ics are now being sold with lead free pin tin. Normal solder does not want to wet out on the pins very well. This silver solder works like a champ on a 700F degree solder station.

Gary
--

[Quacker]

I see. I thought you were referencing a "silver solder." Sorry about that.

I'm just starting to look at RoHS so I'm not yet up to speed on lead free.

The DHL guy just dropped off a package. Guess what? Two samples from MEMSIC!
One each of:
MXR2999
MXR7202

[Gary Warner]

The DHL guy just dropped off a package. Guess what? Two samples from MEMSIC!
One each of:
MXR2999
MXR7202


Frassin, rackin, rrrr, rokin… :censored: :censored: :censored:

I've got to work on my begging skills :D

BTW, Eagle has the package for that. I found it under Analog Device's ADX202 (LCC-8). It's the only pre-defined package on Eagle that I could find.

Gary
--

[Gary Warner]

I see. I thought you were referencing a "silver solder." Sorry about that.

It's what we call it in my industry, but that's not to say it's correct :cool:.

Gary
--

[Quacker]

Which one should I try first?

[Gary Warner]

Which one should I try first?

Wat cha gona do wit it?

Gary
--

[Quacker]

Jam it (through any buffering, gain, etc. required) into the analog input of an FMA FS8 receiver. As a bonus the FS8 outputs 3VDC.

I guess I was asking what the useful "G" range I should be looking at would be.

[Quacker]

BTW, anyone make a breakout board?

[Gary Warner]

Well, I'd go for the 2G unit. 1G seems a bit too sensative for most airborn projects, but then again...

You'll find that these sensors have outputs at a greater scale than advertised. I don't know how accurate the output is outside published scales, but my 2G PWM output version is usable to about 3.75Gs.

Gary
--

[Gary Warner]

BTW, anyone make a breakout board?

I haven't seen any. The LCC-8 doesn't seem to be a popular package. Looks like you'll be etching PCB's tonight :p.

Gary
--

[Quacker]

Thanks Gary. Are you saying that small yaw errors generate enough force so that it easily registers on the 2G unit, or that the 1G unit gets swamped by other transient forces?

[Quacker]

Gary,

'Found this board over at sparkfun. Looks like it's a fit and correct pinout.

http://www.sparkfun.com/commerce/product_info.php?products_id=624

[Gary Warner]

Thanks Gary. Are you saying that small yaw errors generate enough force so that it easily registers on the 2G unit, or that the 1G unit gets swamped by other transient forces?

Oh, no. Not the yaw forces. It's the vertical G forces (if you are refering to the Hamster). The yaw forces seem to fit nicley into the 2G range. But I can't tolerate just 2 Gs of vertical forces, seeing how 1 G is already the norm. That's just a 1 G working range that's left. Makes G force removal on the yaw axis impracticle. That's why I've gone to 10 G's. (5 G's would fit nicley, but they don't have one in the PWM version).

Uh, why you want to know ;).

Gary
--

[Gary Warner]

Gary,

'Found this board over at sparkfun. Looks like it's a fit and correct pinout.

http://www.sparkfun.com/commerce/product_info.php?products_id=624

Bingo! Its even got the ground plane under the sensor. Nice find.

Gary
--

[Quacker]

I had assumed that the sensor would be oriented so that the output was nulled when no yaw force was present. Then a left/right yaw would produce +/- from center. If it is nulled, won't additional G force in the same axis be ignored or am I not understanding something?

[Gary Warner]

I had assumed that the sensor would be oriented so that the output was nulled when no yaw force was present. Then a left/right yaw would produce +/- from center. If it is nulled, won't additional G force in the same axis be ignored or am I not understanding something?

Yaw force errors will be realized if there is some degree of yaw error and vertical G forces change. If there is no yaw error, then right, vertical G forces won't affect the yaw axis readings. Real world, vertical G forces are most always changing and some degree of yaw will most always be sensed. This means that the amount of read yaw error will be wrong.

Gary
--

[Quacker]

Gary,

I'm not trying to nitpick this, just understand the error terms. If I understand you, the vertical G force to yaw signal coupling is an effect of perhaps axis misalignment? Assuming a large vertical G and small yaw signal, perfect alignment (and therefore rejection of vertical G force) is unavoidable. Is this correct?

[Gary Warner]

Gary,

I'm not trying to nitpick this, just understand the error terms. If I understand you, the vertical G force to yaw signal coupling is an effect of perhaps axis misalignment? Assuming a large vertical G and small yaw signal, perfect alignment (and therefore rejection of vertical G force) is unavoidable. Is this correct?

It has nothing to do with axis misalignment.

Think about it for a minute. Perceived gravity is a single vector. It points in only one absolute direction at any given time. If the vector does not align its self exactly perpendicular to one axis or the other, both axes will be effected. Understanding this is only one step in resolving the correct amount of yaw. You also have to resolve gain issues based on dynamic G forces that can change from -10 G's to +10 G's. So the vector angle has to be resolved and the gain of that vector has to be resolved, then the resulting data can be used to calculate the true amount of yaw.

Are you trying to make your own Hamster?

Gary
--

[Quacker]

So Gary,

It seems to me that if the sensor axis of sensitivity is aligned exactly perpendicular to the axis of interest (in this case, the yaw axis) and parallel to the bank axis, that varying amounts of g-force in a perfectly coordinated turn will not register. If however, the turn is not coordinated an error term will emerge from the senor that is proportional to the cosine of the bank angle error. The magnitude of the sensor output for a given angle error would be directly proportional to the magnitude of the g-forces in play. That's another way to say that if the plane is in a high g turn, smaller angular errors will cause higher sensor response. With the gain of this error term as the only variable for the control loop, the loop response can be modeled to be stable over a wide range of gains by shaping the frequency response to assure a 6dB/Octive roll off. My point in describing this is that once this is accomplished, the control loop will attempt to resolve the error term to zero by applying whatever rudder is necessary. In this scenario, there is no need to calculate the gain term and apply precisely the correct amount of rudder, since the loop gain will take care of this automatically. In short, this would be about the same as any closed loop control system.

I have all the parts to build one, so perhaps I’ll get into it. My version would be easy since I use an FS8 receiver that takes analog inputs and the loop gain can be adjusted in flight from the ground. Since the FS8 is set up to correct bank angle, I would likely apply bank correction instead of rudder.

[Gary Warner]

So Gary,

It seems to me that if the sensor axis of sensitivity is aligned exactly perpendicular to the axis of interest (in this case, the yaw axis) and parallel to the bank axis, that varying amounts of g-force in a perfectly coordinated turn will not register. If however, the turn is not coordinated an error term will emerge from the senor that is proportional to the cosine of the bank angle error. The magnitude of the sensor output for a given angle error would be directly proportional to the magnitude of the g-forces in play. That's another way to say that if the plane is in a high g turn, smaller angular errors will cause higher sensor response. With the gain of this error term as the only variable for the control loop, the loop response can be modeled to be stable over a wide range of gains by shaping the frequency response to assure a 6dB/Octive roll off. My point in describing this is that once this is accomplished, the control loop will attempt to resolve the error term to zero by applying whatever rudder is necessary. In this scenario, there is no need to calculate the gain term and apply precisely the correct amount of rudder, since the loop gain will take care of this automatically. In short, this would be about the same as any closed loop control system.

I have all the parts to build one, so perhaps I’ll get into it. My version would be easy since I use an FS8 receiver that takes analog inputs and the loop gain can be adjusted in flight from the ground. Since the FS8 is set up to correct bank angle, I would likely apply bank correction instead of rudder.
Very good. You are the first person I've seen here that can echo back to me in there own words a complete and full understanding of what it is I'm doing. I'm impressed. Only I don't follow the "by shaping the frequency response to assure a 6dB/Octive roll off" thing.

On the PCB's, they were sent out to me. But, unfortunatly they are stuck in China for a week long national holiday. The shipper does not move anything during this holiday. I'll get them next week.

Gary
--

[Quacker]

Well... A closed loop control system is the first cuisine of the oscillator. The only real difference is the number of degrees of phase shift that accumulate around the loop. If the phase shift is 360 degrees or more at a given frequency, and the loop gain at that frequency is more than 1, it will oscillate. If less, it will be stable. Most control loops strive for as much less as practical for best stability and dampening. This is called “phase margin.” Given that it is a closed loop, there is by definition already a 180 degree shift because an error in one direction causes a correction in the opposite direction (180 degrees out of phase). There is also by implication, significant loop gain. If not for this, the loop could not reduce the error term. (A loop gain of 2 would only reduce the error term by half). To do a good job over a range of sensor responses (bulk g-forces) you might like a gain of 10 or 20, reducing the error to negligible amounts. Additional phase shifts that add to the 180 degrees occur as a function of frequency. These include the inertia of the aircraft in the axis the loop will be acting on, and the circuit response time which includes sensor frequency response, filter response, program cycle time (e.g. transport delay), etc. If the addition of all these delays come anywhere near to 360 degrees, and if the loop still has a gain more than 1 at that frequency, you have made a nice wing or tail wager. Since it’s desirable to reduce the error term (that’s the point of this project) it makes sense not to limit the loop gain too much or the goal won’t be met. A good thing to do is to shape the frequency response of the loop to push back against some of the accumulating phase shift. A good example might be if you crank up the gain in an attempt to improve accuracy but observe a 2 Hz wiggle in the rudder. If you can include a 2 Hz “feed forward” (think opposite of a filter), it will compensate for the wiggle and if done properly, will stop it.

I realize that I didn't directly answer your question about 6Db/Octive. This is the rate of gain reduction as frequency increases, for any one simple filter (like an R/C). Such an element has a maximium phase lag contribution of 90 degrees. If the loop gain is rolling off with frequency and crosses the unity gain point roling at 6Db/Octive, the loop is very likely stable. 180 pluse 90 = 270 degrees, or a phase margin of 90 degrees: you win. A higher roll off rate implies that phase shift is accumulating rapidly and that oscillation is very likely.

[Gary Warner]

Ok, I see what you are saying. For now, the Hamster has moved forward with just adjusting gain to control oscillations and LUTs for rate control. I was in the middle of working this out when I discovered that the changes in G’s were causing the gain to change too much. I always knew it was changing the gain, I just didn't realize just how much. So the last prototype I was able to remove most of the gain issues from changing G's by using the second axis. It's not perfect because I don't consider forward/back acceleration. It did make a huge improvement in gain stability for a given airspeed in a thermal-turn. The optimum answer would include airspeed feedback(edit: and rate gyro), but this would negate a prime objective of the Hamster; a drop-in yaw management solution. This is where I've left off.

The next code improvements will be in the user programming and in fine tuning the LUT for deviation rate. I also want to consider and experiment with bi-directional rate routines (one for increasing errors and one for decreasing errors instead of the LUT). I'm not sure if the latter will be in the next production run or that I'll ever finish fine tuning the Hamster. This seems to be an ongoing experiment that has no foreseeable final ending.

Your last post was good reading. Thanks for sharing.

Gary
--

[Gary Warner]

Hey Q,

While we are talking about this stability thing, what do you think about this?

When I was working on the AOA system, oscillations were a big pain. I abandoned the project years ago, but this was an idea I had at the time to help reduce the oscillations. It's the bi-directional gain idea.

[Quacker]

Thanks. It's a voluminous subject and this is just a quick glance.

I would guess that most gliders oscillate at nearly the same frequency for a given wingspan. If so, it may be practical to introduce a simple "feed forward" also known as a "zero" into the loop and fix it for all airspeeds and gliders. If you're game, we could hack on this together offline. It might relieve your concerns about universal adaptability.

Q

[Quacker]

Looks like we cross posted. While gain compensation can work, so can frequency compensation, since it takes both gain and frequency response to cause oscillation. The potential benefit of frequency compensation is that most frequency determining stuff doesn't move that much, so a simple fix will usually work for most cases. Gain compensation can be much more challanging.

[Gary Warner]

Thanks. It's a voluminous subject and this is just a quick glance.

I would guess that most gliders oscillate at nearly the same frequency for a given wingspan. If so, it may be practical to introduce a simple "feed forward" also known as a "zero" into the loop and fix it for all airspeeds and gliders. If you're game, we could hack on this together offline. It might relieve your concerns about universal adaptability.

Q
I would say from observations that the frequency of yaw increases with reduced mass. Less mass about the yaw axis has a higher frequency. This might be a challenge to make the Hamster for hand launch gliders and open class gliders. Then again, the lead-in frequency could be user programmable for a range of sailplanes.

Thinking... :rolleyes:

Gary
--

[Quacker]

Pretty good bet. Your oscillation frequency observations confirm my suspicions.

[Gary Warner]

As I sit here thinking about the 'frequency' issue I realize that there are ranges of frequencies that are speed dependent. I can get my sailplane to yaw (wag-its-tail) very quickly at high speeds. The frequency can be on the order of 3 or 4 times that of slow thermaling speeds. I think the assumption that the yaw frequency is somewhat stable might not be found to be true.

By the same considerations, gain also increases with speed.

I just can't "see" in my head a one-fits-all solution. I think both issues would need to be addressed in parallel. And I can't get there without information about airspeed.

Before someone reads this without haven followed the Hamster saga, the Hamster has next to no issue with oscillations when used for improving thermaling. It's the 100MPH showboat dives I'm talking about.

Gary
--

[Gary Warner]

Oh, and before I forget, I was considering using a rate gyro coupled in series with the AOA sensor system to facilitate the bi-directional idea. This was because I was coding in asm and advanced math was beyond my abilities. But, as I said, I never flew any solution to the oscillations.

[Quacker]

As I sit here thinking about the 'frequency' issue I realize that there are ranges of frequencies that are speed dependent. I can get my sailplane to yaw (wag-its-tail) very quickly at high speeds. The frequency can be on the order of 3 or 4 times that of slow thermaling speeds. I think the assumption that the yaw frequency is somewhat stable might not be found to be true.

By the same considerations, gain also increases with speed.

I just can't "see" in my head a one-fits-all solution. I think both issues would need to be addressed in parallel. And I can't get there without information about airspeed.

Before someone reads this without haven followed the Hamster saga, the Hamster has next to no issue with oscillations when used for improving thermaling. It's the 100MPH showboat dives I'm talking about.

Gary
--


I'm wondering if the oscillation speed increase you observed was actually an amplitude increase. Chances are good that it was varying in amplitude more than frequency. Perhaps this needs looking into.

As for a rate gyro, yes that will do good things because it's a trend sensor, meaning that it's contribution is a lead or feed forward, gaining back 90 degrees. I think the same data could be teased out of the accelerometer wthout the gyro since the rate of data change is also proportional to the rate of yaw change.

[Gary Warner]

I think the same data could be teased out of the accelerometer without the gyro since the rate of data change is also proportional to the rate of yaw change.

That was my thoughts. I've come a long way in what I can code and it's possible now. This is a 'bit' of what I have done with the Hamster, but it's limited due to the code overhead of rate averaging. I use a 'sliding window' of sorts to control fast moving errors and the gain used to correct that error. It's a bit crude, but it works. Admittedly I could do much better with time and testing.

I know I can get a faster cycle of yaw from a faster plane, but this really has little to do with oscillations centering over "0" yaw. What I'm doing is changing the energy level of yaw axis rotation by moving the rudder. More speed, more energy, faster swings. It's different than 'natural' yaw resonance that I think you are referring to.

With the advent of these new $80 5 ounce 'pod' flash-card camcorders I can now strap one on a sailplane looking back to 'see' the rudder response and a piece of yarn at the same time. I've got one on order and expect to make some good progress with the fine tuning process.

This is good brain food. It's got me thinking again. Perfection is always a good goal, but almost never reached.

Gary
--

[Quacker]

That was my thoughts. I've come a long way in what I can code and it's possible now. This is a 'bit' of what I have done with the Hamster, but it's limited due to the code overhead of rate averaging. I use a 'sliding window' of sorts to control fast moving errors and the gain used to correct that error. It's a bit crude, but it works. Admittedly I could do much better with time and testing.

I know I can get a faster cycle of yaw from a faster plane, but this really has little to do with oscillations centering over "0" yaw. What I'm doing is changing the energy level of yaw axis rotation by moving the rudder. More speed, more energy, faster swings. It's different than 'natural' yaw resonance that I think you are referring to.

With the advent of these new $80 5 ounce 'pod' flash-card camcorders I can now strap one on a sailplane looking back to 'see' the rudder response and a piece of yarn at the same time. I've got one on order and expect to make some good progress with the fine tuning process.

This is good brain food. It's got me thinking again. Perfection is always a good goal, but almost never reached.

Gary
--


An onboard observer could be a real advantage!

Is the sensor on the same board with the PIC? I can imagine that an opamp with some frequency shaping components between the sensor and PIC would be one way to get the function stuffed in there without the coding overhead. A small pot here or here to adjust things and when the dust settles, you could attempt to remove the amp and insert the code.

Just a thought...