EAGLE Central Forums
Where the EAGLE community meets. Sponsored by Stratford Digital.

Home » EAGLE Related Forums, Blogs, ... (Read-Only) » Element 14 :: EAGLE Related Posts » Atmega328 - Newbie design (Element 14 :: EAGLE Related Posts)
Atmega328 - Newbie design [message #166759] Sat, 27 August 2016 06:42 Go to next message
messages@element14.co
Messages: 380
Registered: March 2013
Senior Member
Hi All, A little new to the Eagle PCB, so please bear with my silly questions. I had designed a single sided board and all ready for etching. Printed the circuit on paper, only to find out that ATmega328 does not fit in the printout. Download all available libraries of eagle and non seem to be working.  Any help would be appreciated.Original article at https://www.element14.com/community/message/204609?tstart=0#204609.

-- Web access to CadSoft support forums at www.eaglecentral.ca. Where the CadSoft EAGLE community meets.
Re: Atmega328 - Newbie design [message #166760 is a reply to message #166759] Sat, 27 August 2016 07:43 Go to previous messageGo to next message
messages@element14.co
Messages: 380
Registered: March 2013
Senior Member
Are you sure that your printer is printing at exactly 1:1 ratio - check the board overall dimensions to scale the printer. MKOriginal article at https://www.element14.com/community/message/204629?tstart=0#204629.

-- Web access to CadSoft support forums at www.eaglecentral.ca. Where the CadSoft EAGLE community meets.
Re: Atmega328 - Newbie design [message #166761 is a reply to message #166759] Sat, 27 August 2016 08:40 Go to previous messageGo to next message
messages@element14.co
Messages: 380
Registered: March 2013
Senior Member
All were working earlier. now all of a sudden its happening. I've also re-installed eagle. Below is the dimensions in mmOriginal article at https://www.element14.com/community/message/204610?tstart=0#204610.

-- Web access to CadSoft support forums at www.eaglecentral.ca. Where the CadSoft EAGLE community meets.
Re: Atmega328 - Newbie design [message #166762 is a reply to message #166759] Sat, 27 August 2016 11:34 Go to previous messageGo to next message
messages@element14.co
Messages: 380
Registered: March 2013
Senior Member
So when you print it what does the 109.22 dimension actually measure with a ruler ? MKOriginal article at https://www.element14.com/community/message/204641?tstart=0#204641.

-- Web access to CadSoft support forums at www.eaglecentral.ca. Where the CadSoft EAGLE community meets.
Re: Atmega328 - Newbie design [message #166763 is a reply to message #166759] Sat, 27 August 2016 12:52 Go to previous messageGo to next message
messages@element14.co
Messages: 380
Registered: March 2013
Senior Member
That's a horrible layout (in my opinion). Did an autorouter do it? If the primary of your transformer has mains on it, you need much better spacing there than the minimum default setting. The ground layout on the secondary side could be much better too. Having the output cap for the regulator up next to the switches at the top seems like an odd placement. You might also want to increase the widths of the tracks (for current handling ability) around the load switch and the snubber components. The isolation figure for the opto device controlling the triac is meaningless if you push tracks from the low voltage side between the pins on the high voltage side. If you have to have a single-sided layout, perhaps consider a few wire links on the top rather than the very convoluted paths on the bottom layer. Sorry if that sounds like a bit of a brutal critique. It's meant to be helpful (so you can improve the layout) rather than stop you in your tracks (so to speak).Original article at https://www.element14.com/community/message/204561?tstart=0#204561.

-- Web access to CadSoft support forums at www.eaglecentral.ca. Where the CadSoft EAGLE community meets.
Re: Atmega328 - Newbie design [message #166764 is a reply to message #166759] Sat, 27 August 2016 13:31 Go to previous messageGo to next message
messages@element14.co
Messages: 380
Registered: March 2013
Senior Member
Hi Jon! Yes, that's a typical output from its auto-router. You soon recognise the 'style' of its output : )Original article at https://www.element14.com/community/message/204634?tstart=0#204634.

-- Web access to CadSoft support forums at www.eaglecentral.ca. Where the CadSoft EAGLE community meets.
Re: Atmega328 - Newbie design [message #166765 is a reply to message #166759] Sat, 27 August 2016 13:48 Go to previous messageGo to next message
messages@element14.co
Messages: 380
Registered: March 2013
Senior Member
Thanks guys for the feedback. Am just getting starting, taking those baby steps. Figured the printout size, it was the generic driver that the printer had. Changed it to the recommended driver and all works well. Was gonna etch it today. Will hold it back.Original article at https://www.element14.com/community/message/204565?tstart=0#204565.

-- Web access to CadSoft support forums at www.eaglecentral.ca. Where the CadSoft EAGLE community meets.
Re: Atmega328 - Newbie design [message #166766 is a reply to message #166759] Sat, 27 August 2016 13:50 Go to previous messageGo to next message
messages@element14.co
Messages: 380
Registered: March 2013
Senior Member
You're absolutely right - I was just responding to the dimension issue and I didn't look at the circuit itself. @George, Google "ipc mains clearances" - you'll get lots of hits which will give some idea as to what a board with mains on it should look like.  Before you do put mains on your own pcb do please post it here again - for more good, if tough, advice. MKOriginal article at https://www.element14.com/community/message/204643?tstart=0#204643.

-- Web access to CadSoft support forums at www.eaglecentral.ca. Where the CadSoft EAGLE community meets.
Re: Atmega328 - Newbie design [message #166767 is a reply to message #166759] Sat, 27 August 2016 13:52 Go to previous messageGo to next message
messages@element14.co
Messages: 380
Registered: March 2013
Senior Member
Hi Jon, Would you be having a documentation or provide me some tips to place the components. I have downloaded the autoplace_v3.ulp to see it can help but that returned an error "access open c:\windows\system32\place.scr". Any idea how i can resolve this.Original article at https://www.element14.com/community/message/204657?tstart=0#204657.

-- Web access to CadSoft support forums at www.eaglecentral.ca. Where the CadSoft EAGLE community meets.
Re: Atmega328 - Newbie design [message #166768 is a reply to message #166759] Sat, 27 August 2016 15:09 Go to previous messageGo to next message
messages@element14.co
Messages: 380
Registered: March 2013
Senior Member
So far I've got this from what I could gather reading. Maybe not best placement but would this be ok.Original article at https://www.element14.com/community/message/204635?tstart=0#204635.

-- Web access to CadSoft support forums at www.eaglecentral.ca. Where the CadSoft EAGLE community meets.
Re: Atmega328 - Newbie design [message #166769 is a reply to message #166759] Sat, 27 August 2016 15:30 Go to previous messageGo to next message
messages@element14.co
Messages: 380
Registered: March 2013
Senior Member
[I wrote this quickly before seeing your subsequent post, so this refers to your first layout.] Sorry, I realise I didn't phrase that very well. I was referring to the track layout - the component placement isn't all that bad. Parts are mostly where they need to be with some exceptions. Remember I can't see your circuit and I'm reconstructing it in my head from the layout. The capacitor on the output of the bridge rectifier needs to be right there at the output. Perhaps make it a 5mm pitch part (or bend the legs of a 2.5mm part to fit a 5mm placement). It looks like the crystal and its load capacitors are on the wrong side of the processor. The tracks to the crystal should be short. It doesn't look like there's a decoupling cap for the processor - certainly not one in the right place (next to the supply pin) What are the resistors with the links doing? They don't seem to be pull-ups. Are they necessary? Imagine a line 5mm wide drawn vertically up through the centre of the opto driver for the triac the full height of th eboard. Try and get all the mains stuff on one side and all the low voltage stuff on the other and nothing on the line. Think of it as a moat that nothing can cross except the transformer and opto driver acting as bridges. That gives you a reasonable minimum level of primary to secondary isolation on the board. Move the PLED connector across so that it's not with the mains stuff. I'd use a wider pin pitch than 2.54mm for the AC and LOAD connectors. 3.95(?) or 5.12 would be better. On the mains side go for as much clearance as possible. You certainly don't want the situation where the tracks wind round the connectors with 0.15mm or 0.2mm spacing. The situation with the triac, where the track from the top pin slopes down and comes to within the minimum spacing of the centre, is out too.  To get a sensible track layout for something like this you need to do it by hand. What is the fuse rating of the load circuit? That tells us the maximum continuous current and we can then tell you the minimum track width you'll need to carry it. Original article at https://www.element14.com/community/message/204658?tstart=0#204658.

-- Web access to CadSoft support forums at www.eaglecentral.ca. Where the CadSoft EAGLE community meets.
Re: Atmega328 - Newbie design [message #166770 is a reply to message #166759] Sat, 27 August 2016 15:49 Go to previous messageGo to next message
messages@element14.co
Messages: 380
Registered: March 2013
Senior Member
wow that was a mouth full . So to understand. I need to separate the mains AC from the dc side. GOT IT ! About the resistors, which one ? the AC mains is 240v with a 5amp fuse in it. The PCB transformer is rated at 9v 1.5VA. This is the below circuit.Original article at https://www.element14.com/community/message/204636?tstart=0#204636.

-- Web access to CadSoft support forums at www.eaglecentral.ca. Where the CadSoft EAGLE community meets.
Re: Atmega328 - Newbie design [message #166772 is a reply to message #166759] Sat, 27 August 2016 18:37 Go to previous messageGo to next message
messages@element14.co
Messages: 380
Registered: March 2013
Senior Member
I thought the devices down the board were selection links. They're LEDs, so of course you need the resistors. To carry 5 amps, at 25C, on a board with 1oz copper, with no more than a 10C temperature rise you need a track width of something like 2.8mm (that applies whatever the voltage). However a fuse doesn't blow at the rated current (at least not quickly - look in a datasheet which will have a graph of time-to-blow against current), so you would do well to increase that to cover more than 5A. If you want to see how current varies with track width there are plenty of track width calculators online. I can't go any further than this with the mains side. It's not something that I normally do and I'm not qualified to hand out advice as to how it should be done (I know what you shouldn't do, but I'm less clear on what you should do). In particular, I can't advise you on the clearances you need. I know it gets complicated, because it includes making judgements about factors like the environment the board will be in, and being careful to distinguish clearance (the distance through the air between two conductors) and creepage (the distance along a surface between two conductors) which may have different ratings. Are you sure you really need to be doing the mains layout? Can you not do what you want to do with a PSU and a solid state relay?Original article at https://www.element14.com/community/message/204621?tstart=0#204621.

-- Web access to CadSoft support forums at www.eaglecentral.ca. Where the CadSoft EAGLE community meets.
Re: Atmega328 - Newbie design [message #166777 is a reply to message #166759] Sun, 28 August 2016 19:54 Go to previous messageGo to next message
messages@element14.co
Messages: 380
Registered: March 2013
Senior Member
First off, uncheck the scale to fit box as shown below to get a true 1:1 printout. Original article at https://www.element14.com/community/message/204689?tstart=0#204689.

-- Web access to CadSoft support forums at www.eaglecentral.ca. Where the CadSoft EAGLE community meets.
Re: Atmega328 - Newbie design [message #166871 is a reply to message #166759] Sat, 03 September 2016 16:11 Go to previous message
messages@element14.co
Messages: 380
Registered: March 2013
Senior Member
nope it was not. It was the driver of the printer that had the generic rather the manufaturers recommended driver. installed the driver and all worked well.Original article at https://www.element14.com/community/message/205013?tstart=0#205013.

-- Web access to CadSoft support forums at www.eaglecentral.ca. Where the CadSoft EAGLE community meets.
Previous Topic: E112-J112 Eagle library
Next Topic: How do I get an always uptodate rats nest?
Goto Forum:
  


Current Time: Fri Apr 28 19:57:10 GMT 2017