Hi Guys,
I have just created my first schematic and layout in the cadsoft eagle software!!
Isnt as bad as I thought but could a few of you take a glance over the work for any obvious errors and improvements?? ???
The pedal is a combined SHO and Wolly Mammoth with separate in's and out's.
(http://i791.photobucket.com/albums/yy196/craigmillard/mammothhardonschem.png)
(http://i791.photobucket.com/albums/yy196/craigmillard/mammothhardon.png)
Cheers
Craig
Wow, looks much better than my first one. A few things:
1) Make sure you have thermals on for your ground plane pads
2) Lug 2 of the crackle pot currently isn't connected to anything because you don't have a little green dot on the schematic to where it connects to lug 1 and R11. Put a dot there and it should be easy to just add a track to lug 1 on the layout.
3) I don't have the schematic, but I just want to make sure that R2 connected to the pinch knob isn't supposed to be connected to the emitter and ground of Q1. I don't think it would be, but since those little green dots are a pain to remember, I thought I'd make sure.
For a first Go I would say you did a smash up job. I just started using designspark PCB. its very similar to Eagle but their is no size limitations and the library's are a lot easier to manage. I still prefer Eagle due to the mouse zoom is a lot smoother but I think the dimension limitation overcomes that drawback.
You'll want thermal isolation on your ground pads if you don't already have them. Cant' tell from the pic.
You can probably negotiate the layout to get rid of the jumper to that lower cap. Not sure if you could eliminate the other two jumpers.
cheers mth5044
Good spot on the green dots!:) R2 isn't ment to connect to the emitter so that one is correct but the lug 2 was wrong although in the layout it would have been fine! :icon_biggrin:
regarding the thermals, not sure how to do that? What does it involve??
Quote from: craigmillard on November 17, 2010, 10:26:04 AM
cheers mth5044
Good spot on the green dots!:) R2 isn't ment to connect to the emitter so that one is correct but the lug 2 was wrong although in the layout it would have been fine! :icon_biggrin:
regarding the thermals, not sure how to do that? What does it involve??
Haha, this took me way to long to figure out, and I think I had a thread were many people were helping me, but I think I got it down now :icon_confused: You have to change the >NAME or whatever of the polygon that you are using for ground to GND or whatever you grounding scheme is named on the schematic. I don't remember how exactly to do that because I don't have my computer with EAGLE on it infront of me, but I think you can just go to info and change the name. Then make sure thermals are on (under DRC or ERC or some button that has three letters).
You can also run a design rule check (I think that's what it's called, DRC) to make sure the program likes everything you did (layout matches up with schematic, everything's connected, etc).
yup i have set the poly NAME to my GND name and set the tick box for thermals in the DRC checker:) I assume that is all that is required!?
I have found a couple of other issues though:
1. the pads in the ground plane are not completely surrounded? only small connections on 4 sides?
2. The DRC Checker is saying clearance on the transistors are too small and drill sizes are wrong, how can I enlarge these? I have used the Gausmarkov librarys, is this something to do with these?
Thanks
Craig
Go to the DCR, click the supply tab. Those are all of the parameters if you need to adjust them. But the thermal should show up if you change the Width parameter of your pour outline. This is the tutorial I used when I was learning this stuff. http://gaussmarkov.net/wordpress/tools/software/eagle/ground-pour/5/
Quote from: craigmillard on November 17, 2010, 11:04:30 AM
1. the pads in the ground plane are not completely surrounded? only small connections on 4 sides?
Those are the thermal pads. By carving out copper from around the pad you make it a lot easier to heat up the pad with the iron, rather than trying to heat up the whole ground plane.
Just read Gausmarkov's guide and twigged that this is how the thermals are meant to be! :icon_lol:
The drill sizing and spacing I think I am OK to ignore as the printed layout looks fine to the eye with no traces touching and plenty of distance between the pads!
Cheers Guys, think I may give this an etch and see how it goes then! 8)
Ok, stared at it some more. Layouts are like crack to me. Way more fun than sudoku and I get something in the end. Your layout is fine as it is, these are just tweaks and tricks I use.
Swapping the positions of C1 and Q2 will get rid of one of the jumpers.
Moving the cap right up against the EQ pot, I think it's C2, to the right will allow you to route under R3 (?) and C2 and allow you to get to the outside lug of the EQ pot. That gets rid of the last jumper.
The pots aren't close enough to the edge of the board if you're going to mount them like that. If you move them forward, you may run into problems with the EQ to Level trace violating the trace to edge parameter in the DCR. There are a couple of ways to deal with that, though reducing the trace width is one work around. Moving the pots will screw up your ground pour.
Putting jumper pads under the pot casing will make getting to that pad a pain in the a$$.
You can eliminate two of the three jumpers you have in there. Move C3 downwards for the first one. You may have to erase the ground plane there.
For the second one, move C5 to the left. Aling its left pad with R5`s pad. If you can, make a straight connection with R4. Now, you should have enough space to place a trace that goes between C5`s terminals cleanly.
If you are planing to mount pots directly to the board as in here http://www.negatron.org/wp-content/uploads/2009/02/onboardpots_342.jpg , make sure you delete all the upper ground plane. Otherwise, the pcb itself is going to touch the box and may stress the pots and finally crack the joints.
In other words, the pcb should end where the pots shaft starts.
You have a very nice layout in there ;)
-----------------------------------------------------------------------------------------------------------------------------
Deadface beat me first ;)
As for moving the pots forward, you could connect the ground from the sides and down side
thanks for the help all!:)
I have re-dun the layout slightly to try and shrink it below the pot shafts and also space the pots out a bit more! :icon_razz:
(http://i791.photobucket.com/albums/yy196/craigmillard/MHO2.png)
As you can see i still have 2 jumpers! :-\ Any ideas?
:icon_biggrin:
(http://img168.imagevenue.com/loc788/th_95306_pcb_122_788lo.jpg) (http://img168.imagevenue.com/img.php?image=95306_pcb_122_788lo.jpg)
The size changes but you don't need jumpers.
That's right! Very good!
You still can remove the first jumper that connect the EQ pot with the Level pot. Just remove the ground plane under those pots and trace the connection as it was before, but you should connect the ground plane down the crackle pot so everything connects together
Just a question - are you planning on making this board yourself? I mean, most (I would think) people make eagle files because they are accepted by most PCB fab places. If you wanted to make PCB's at home, you might be better off going for a simpler layout program? It looks like you have a good hang of eagle so far though..
..but the reason I ask is that you can easily do double sided layouts (or even 4 layer) in eagle and have them fabbed at a house. You can make the layout considerably smaller and get rid of jumpers if you go for double sided. That is the main reason I learned eagle.. double sided layouts + the ability to have houses make them. So, if this isn't to make at home, you can look into double siding it.
Eagle does translate to DIY board work very nicely with a direct PDF output. I do agree, that going double sided and having the boards fabbed makes life much simpler.
For just doing a couple of boards I've had great fun and success with the Dorkbot group board buys - $5 a square inch gets three boards.
http://www.dorkbotpdx.org/wiki/pcb_order
I'll throw a +1 in for dorkbotpdx. Laen's a great guy.
Just a few tips to have in mind:
. When you move a component you should apply the ripup command to the component to change a routed trace back to an airwire, then move it. This way, you can re-route the connection later and have a clean trace.
A clear example of not applying this, is the trace that connects R10 with the 4001 diode.
. In cases like R4, is best to have a straight trace under R4 and then connect it whit a vertical trace. Something like an upside down "T"
. Again, in cases like R6, is best to connect it like a reversed "L".
. The trace from the first pin of the Pinch pot its too long. There is no point (as far as I could see) in having it like that
. The trace that connects Q1c with Q2b should also join like a "T". This way, you can use closer distance pins for C4
. You can have C3 placed between R2 and C2 (moving them a little), sou you can save the last jumper.
Thanks alot everyone, think i have a finished board now:)
(http://i791.photobucket.com/albums/yy196/craigmillard/MHO3.png)
(http://i791.photobucket.com/albums/yy196/craigmillard/mho3u.png)
Gotta say SISKO & defaced, you have been a great helps! :icon_biggrin:
Now have the board fitting in a 1590BB Width and height, with some strategic placing it may even go into a 1590B :P
This is just for home etching at the moment but liked the idea of getting to know how to use eagle in the possibility I may run off some fabbed boards!:)
The gaussmarkov librarys and guides are a great help for anyone wishing to learn, thankyou gaussmarkov!!
Looks good! The more you play with Eagle or any PCB software, the more you'll learn about board layouts and how to do them.
One thing that will kill you with board houses, is your name and text in the copper. Depending on the rules the house uses, they will kick your design because text usually violates minimum clearance limitations/sizes. This caused me alot of heartache about a year ago when I was doing a large board order.
Nice work! Also, D2 is backwards in the schematic.
Cheers Bean had completely missed that! ::)