Toaster Reflow oven project, need a more experienced eye!

[CrabxCore]

Hello Everyone!

Long time viewer of Daves youtube channel. I recently joined the forums and have been lurking and replying to what I feel qualified to answer. 

Anyways, I am working on building a reflow oven from a toaster oven. It will use an arduino Mega as the main processing power. I have a "shield" designed and a pcb routed, however I am a novice at circuit design and layout. All I know I have learned mainly from experimenting and watching youtube videos. I would really appreciate it if the fellow forum members that have more experience than myself could take a look and call out all my design flaws. I am going to upload my .brd and .sch files in a .rar archieve. All these programs are freeware so everyone has the opportunity to  take a look if they would like to.

A little more about the shield:

Uses 3 K type thermocouples to sense different areas of board.
Uses 3 max31855 cold junction compensation IC's
Uses 1 max3002 for level shifting from 5v to 3v3
Has outputs for 2 Solid state relays, for independent top and bottom element control
Has 2 RBG led's for Status and quick temp check (red if above setpoint, green if within setpoint margin, blue if below setpoint)
Uses a 16 key, 4x4 matrix for input
Uses 2x16 LCD for UI

Things I would like to add in later revisions:
SD card data logging
Additional display capabilities
MatLab data generation (Very far off  )

Thank you in advance for any help!
 --Crab

Can't attach .rar so here is a link on google docs:: https://drive.google.com/file/d/0Bz8gx9yr3X1qR29WWmx5cnROVTQ/edit?usp=sharing

[TheRuler8510]

I want to build a reflow oven for myself also, so I'd love to check out your design, however I can't seem to access your upload.

Do you have a LCD with graphics for a plot?

[CrabxCore]

Hey sorry about that, lets see if this works better.

Attached is a .zip file

**Do you have a LCD with graphics for a plot?**

No I only have a 2 row by 16 column LCD. In theory it could be used to plot the temp but it would have very low resolution on the vertical scale. Currently I am planning on using it to input my profile and view temperature and time data.

[CrabxCore]

Could really use a quick look over by anyone experienced with PCB design. I will be ordering PCB's next week.

[TheRuler8510]

Could really use a quick look over by anyone experienced with PCB design. I will be ordering PCB's next week.

I am looking at it in Eagle. I don't see wrong with it, but I am hardly an expert at Eagle. I am more of a KiCad guy.

What's your main concern? Dimensions? Ground planes?

[mjkuwp]

some of the drilled holes for the vias are 0.015".  Have you checked that with the pcb manufacturer?  seems a bit small but I am also a beginner having done only around  a dozen designs.  I have used down to .023".

I did DRC and the only thing that came up are a bunch of stop mask errors where the silkscreen is overlapping with pads and such.  I don't know technically if this is a problem or not but in that case I usually 'smash' the component and move the text to eliminate that or else I edit the footprint. 

Why are there so many vias around the CON1+, CON2+ and CON3+ ... it is not a criticism just a question.  I have not seen that kind of layout before.

[Tac Eht Xilef]

Could really use a quick look over by anyone experienced with PCB design. I will be ordering PCB's next week.

You're much more likely to get responses if you post or link to images of your schematic & board. Many people here don't use Eagle, few (if any) of them are going to go through a 40meg+ download & install just to take a look, and even those who (like myself) use Eagle aren't going to bother faffing around with downloading & extracting your files on the off chance they can help.

Make it easy for people to give you feedback, and you'll get it in spades...

[CrabxCore]

Could really use a quick look over by anyone experienced with PCB design. I will be ordering PCB's next week.

You're much more likely to get responses if you post or link to images of your schematic & board. Many people here don't use Eagle, few (if any) of them are going to go through a 40meg+ download & install just to take a look, and even those who (like myself) use Eagle aren't going to bother faffing around with downloading & extracting your files on the off chance they can help.

Make it easy for people to give you feedback, and you'll get it in spades...

I will do that now! Thank you for the tip, I don't know why I assumed everyone had EAGLE.

Okay, I have taken screen shots showing all layers on, and only copper layers + via's. Also, I have attached a PDF of my schematic.

Thanks,
Crab

[CrabxCore]

some of the drilled holes for the vias are 0.015".  Have you checked that with the pcb manufacturer?  seems a bit small but I am also a beginner having done only around  a dozen designs.  I have used down to .023".

I did DRC and the only thing that came up are a bunch of stop mask errors where the silkscreen is overlapping with pads and such.  I don't know technically if this is a problem or not but in that case I usually 'smash' the component and move the text to eliminate that or else I edit the footprint. 

Why are there so many vias around the CON1+, CON2+ and CON3+ ... it is not a criticism just a question.  I have not seen that kind of layout before.

I am using OSHpark.com for my PCB's. They list a 13mil min drill size so I went with 2mil over minimum just to be safe. I am also setting my stop mask limit to 16 mil so those 15mil vias will have stop mask on top of them. 

With the stop mask DRC error, I'm not sure if it is a problem either. They state on the website that any silk overlapping a pad will not be printed so I guess I am just hoping they mean in that spot not the entire silk. I will work on getting those errors fixed this week to be safe.

With the Con1+::Con3+ via's, it is a connection for a thermocouple and I was trying to get as much "meat" between the input of the max31855 and the physical connection to keep down the temperature difference. I'm no thermal expert so not really sure if it is going to do much of anything.

Thanks,
Crab

Edit: Attached new .brd with silk errors fixed

[CrabxCore]

Could really use a quick look over by anyone experienced with PCB design. I will be ordering PCB's next week.

I am looking at it in Eagle. I don't see wrong with it, but I am hardly an expert at Eagle. I am more of a KiCad guy.

What's your main concern? Dimensions? Ground planes?

Sorry didn't see your question at the bottom. My main concerns are mainly about conventions on pcb layout. I know it will work electrically, well I hope it will!

Thanks,
Crab

[kizzap]

with the connections on the left, the big boxy looking things, be careful because that leads into the USB, and DC power packs.

Your board outline will be larger then the arduino footprint at the right side of the board. Not sure if that is intentional or not. You can make the dimension layer follow the outline for the mega shield you are using.

As I said in your other thread, you have random wires going through vias for no reason. Drill hits cost money ; )

I would consider if you REALLY need the ISP header cutout. all the pins in that header are already brought up via the pins on the outside headers.

You have ample spare space on that board, there is no reason that you need to dual load at all. (Have components on both sides.)

This is one that many people don't realise: Eagle puts component text down on the PCB as "Proportional" however when you create gerbers for the fab company, Eagle converts the text to "Vector" which actually changes the size of the text. So once you have finished routing the board, smash all your components, and convert all the text to Vector.

Some of your silkscreen labels are 16mil. It is going to not print, or be a single dot. Also i

Your capacitors for filtering the noise on the thermocouple lines is in the wrong place. it needs to literally be next to the IC's pins.

For neatness's sake, try stick to one style of via.

you have your Linear Regs spread all over the place. Move them all to one area to make things neater, and then move them as far away from the Thermocouple measurement areas as possible. I dont know the load on your 3.3V regulator, but you should really consider powering it from the 5V regulator. Even better, the arduino Mega Provides both of those rails, use them and save more space!

That is all I could be bothered finding. Have fun with the respin ;-)

[CrabxCore]

with the connections on the left, the big boxy looking things, be careful because that leads into the USB, and DC power packs.

Your board outline will be larger then the arduino footprint at the right side of the board. Not sure if that is intentional or not. You can make the dimension layer follow the outline for the mega shield you are using.

As I said in your other thread, you have random wires going through vias for no reason. Drill hits cost money ; )

I would consider if you REALLY need the ISP header cutout. all the pins in that header are already brought up via the pins on the outside headers.

You have ample spare space on that board, there is no reason that you need to dual load at all. (Have components on both sides.)

This is one that many people don't realise: Eagle puts component text down on the PCB as "Proportional" however when you create gerbers for the fab company, Eagle converts the text to "Vector" which actually changes the size of the text. So once you have finished routing the board, smash all your components, and convert all the text to Vector.

Some of your silkscreen labels are 16mil. It is going to not print, or be a single dot. Also i

Your capacitors for filtering the noise on the thermocouple lines is in the wrong place. it needs to literally be next to the IC's pins.

For neatness's sake, try stick to one style of via.

you have your Linear Regs spread all over the place. Move them all to one area to make things neater, and then move them as far away from the Thermocouple measurement areas as possible. I dont know the load on your 3.3V regulator, but you should really consider powering it from the 5V regulator. Even better, the arduino Mega Provides both of those rails, use them and save more space!

That is all I could be bothered finding. Have fun with the respin ;-)

Hey kizzap, Thanks for all your help. I'm going to just start over with all of the advice I have received and try to make something that looks more professional.  I will post updated board when I get done

Crab