TheBackShed.com

Forum Index : Microcontroller and PC projects : AutoTRAX DEX Usage Questions

Author

Message

disco4now

Guru

Joined: 18/12/2014
Location: Australia
Posts: 1000

Posted: 01:12am 03 Apr 2015

Copy link to clipboard

Print this post

I have been playing with DEX enough now that I have some questions. My aim is to get to the point of getting a board made for a dual battery monitor I am working on.

So the questions so far. (I have looked at many of the videos)

1. The vias automatically created when you swap from the front to the back layer have a hole of .01 inch. The design rule checker says these should be .015 inch. I cannot find how to change these via holes. Should they be .015 as the design rule says.

2. On the cost of getting the board produced, what parameters affect this, e.g number of layers, number of vias i.e what should you be aiming at.

3. I have an L shaped board. I got this by using a cutout placed in one corner before I looked at the video that showed joining two shapes to get the desired board. This fails the design rules for cutout too close to the edge but board looks OK. Will I be able to use this or will I need to start again.

4. I have some connectors near the edge of the board but pads are slightly closer that .1 inch as flagged by design rules.Are these design rules guiding towards what the board manufacture will accept,is there any leeway.

Thanks
Gerry

Latest F4 Latest H7 FotS

WhiteWizzard
Guru

Joined: 05/04/2013
Location: United Kingdom
Posts: 2933

Posted: 02:25am 03 Apr 2015

Copy link to clipboard

Print this post

Hi Gerry,

In response to questions 2 & 4:

2> Most PCB manufacturers now simply use PCB area for calculating cost (independent of number of components/vias like they use to do) The number of layers is also a cost factor - but if you're design can work on double sided then you can get boards made very cheaply.
If you can keep the design within a 5cm and/or 10cm design area then costs are minimised. So if your board is 4.5cm x 8.9cm then this is good. If its 5.2cm x 8.9cm then alter the layout to try and get the 5.2cm dimension down to 5cm or under.
Shapes/cutouts in PCBs are fine but you will be charged for area based on the maximum x & y dimensions.

4> The design rule checker is just a 'warning' system (all PCB software apps have them). The settings are mainly configurable so sometimes you can vary these values to 'eliminate' annoying warnings.

The best advice I can give is to complete a design, generate the gerbers, and then send it off to a cheap Chinese PCB manufacturer (via their website). I have always strongly recommended iTead as a good place to start. Look for PCB Prototyping, and then select the dimensions that your PCB falls within (i.e. 5x5, 5x10, 10x10). If it is bigger then thats not a problem - just costs a bit more per piece. You will be purchasing 10 'panels' (note that you can put more than one PCB per panel which does then bring down unit cost (as well as you ending up with more than 10 PCBs.

Don't select any 'cost option' finishes (i.e. different colour boards, or different finishes). Simply select from the 'free' options and 'purchase'.

NOTE: Don't think about just buying one PCB - go for their 10panel prototyping service and no options. This will cost you around $20 + shipping. Use DHL shipping (which does double the cost BUT it will still work out cheaper than buying just one PCB from most PCB houses.

Now the main point of all this . . . IF the design doesn't meet their requirements then they will contact you with reasons why. If it does, then you have a bunch of PCBs made. When received (mine take about 11 days from time of order and when using DHL) you can then 'touch & feel' your design. Any 'schoolboy error' can then be corrected in your design and your next order (if required) can be submitted and this time add any cost options (I like to use ENIG finish as it offers much better soldering IMHO - but I would never select ENIG for a 'test' PCB).

Some people I know have said this is a silly approach - but then they have gone for a 'perfect' design for one PCB which costs them (in most occurrences) over �100 PER PCB and then some of the time they get the design wrong! You do the math as to which way is more 'sensible'

Hope this has helped.

PS I have just used a PCB fab house here in the UK for a rapid 5-day turnaround. Two boards were quoted as just under �100 excluding delivery. The Easter weekend is upon us which meant I wouldn't have had the PCBs in my possession until next Wednesday after the Easter holiday. I spoke to them saying I actually needed 39 PCB (not just two) by yesterday (Thursday - being ordered on Tuesday at the start of the week) i.e. a THREE day turnaround. I went to pick up all 39 PCBs yesterday for just over �100

. Supplied them Eagle files (from which they generated the Gerbers), and I had many 'broken' design rules (parts too close to the edges, silkscreens off board, silk overlaps, etc. Result is they done everything and I got exactly what I needed - all boards routed and cutout too.
All other UK PCB Fab houses either couldn't meet my timescales; but if they could, the cheapest quote I got was for �249 for ONE PCB!!!

WW

Edited by WhiteWizzard 2015-04-04

disco4now

Guru

Joined: 18/12/2014
Location: Australia
Posts: 1000

Posted: 02:39am 03 Apr 2015

Copy link to clipboard

Print this post

Hi WW,

Thanks for the good info. Just the info I was after regarding the board manufacture. Just need to finish the DEXing now.

Regards
Gerry

Latest F4 Latest H7 FotS

srnet
Senior Member

Joined: 08/08/2014
Location: United Kingdom
Posts: 164

Posted: 10:06am 03 Apr 2015

Copy link to clipboard

Print this post

I would also have no hesitation in recommending ITDStudio, the boards really are good quality and @ around US$14 delivered for 10 boards, the price is amazing.

They are quite happy to do 6mil tracks and 0.3mm Vias.

Attached is a full size print out of a 40mmx40mm board they did for me, I just checked and there are several tracks within 0.2mm and some pads within 0.1mm of the board edge, no problem.

This particular board has now travelled some 325,000,000KM in rather harsh conditions........

2015-04-03_200435_40x40_PCB.zip Edited by srnet 2015-04-04

$50SAT is Silent but probably still working.
For information on LoRa visit http://www.loratracker.uk/

bigmik

Guru

Joined: 20/06/2011
Location: Australia
Posts: 2949

Posted: 03:52pm 03 Apr 2015

Copy link to clipboard

Print this post

Hi Gerry,

The design rules can be set in the DESIGN RULES CHECKER Panel. Note changes here only reflect the current project.. There are some option settings that should impact new projects but I have found every time an update is done these seem to reset back to default so I usually set them to suit the project and go.

The default auto via seems to be .02" dia with .01" hole I like to use .03" dia and .015" hole I havenmt had any issues with this setting.

Just do your board and then when reasonably happy you can do a global change of your vias and track widths etc in the PROPERTIES Panel (with nothing selected it gives the board properties. then set the desired Via and track widths and click set entire board.

As Phil said most Chinese Fab houses dont care about No of holes.. just the size of the board..

In Dex there are several ways to change the shape of the board.. I have only needed to do it once for a strange shaped board (designed to go into a DB-25 back shell). I did this by double clicking on the boarder and moving the new vertex to where I wanted it to go.. you can then edit each vertex in the properties screen to get them exact, but there are other ways to do it.. If your Gerbers look ok it will be OK.. It may pay to ask the Fab house if the shape will be cut out for you.. it may not..

As for clearances, I am currently working on a board and I have had to resort to tracks .015" from the edge and pads (the edges) about .03" from the edge.. I set my design rules to accommodate them.

Regards,

Mick

PS. Shenzhen2U.com do a decent job for a decent price, turnaround is about 4 weeks for standard snail mail and costs around $21US total for 10 x 10cmx10cm boards if you want DHL total turnaround is less than 2 weeks but will cost around $45-$50US..

Regards,

Mick

Mick's uMite Stuff can be found >>> HERE (Kindly hosted by Dontronics) <<<

Print this page

To reply to this topic, you need to log in.