Page 1 of 1

Eagle Silabs CP2102 library part DRC violation

Posted: Mon Nov 14, 2005 9:51 am
by SmileyMicros
I am trying to use the Silabs CP2102 library part with Eagle and the MLF28 pads cause a DRC clearance violation with the clearance set at 8 mils as per the BatchPCB requirements. Does this mean that this part cannot be used as is? Should I edit the part to make the pads smaller or does the 8 mil rule only apply to routing?

Smiley

Re: Eagle Silabs CP2102 library part DRC violation

Posted: Mon Nov 14, 2005 12:14 pm
by Philba
SmileyMicros wrote:I am trying to use the Silabs CP2102 library part with Eagle and the MLF28 pads cause a DRC clearance violation with the clearance set at 8 mils as per the BatchPCB requirements. Does this mean that this part cannot be used as is? Should I edit the part to make the pads smaller or does the 8 mil rule only apply to routing?

Smiley
same problem as here http://www.sparkfun.com/cgi-bin/phpbb/v ... php?t=1832

edit the part and change the pad width to .29 to get the interpad gap to be > 8 mil.

It would be good if GP would just relax the min gap to .2 mm which is just a tad under 8mil so we can all use the datasheet recommended pad size.

Posted: Mon Nov 14, 2005 1:03 pm
by SmileyMicros
Thanks Philba, I'll just edit the part.

Smiley

Re: Eagle Silabs CP2102 library part DRC violation

Posted: Mon Nov 14, 2005 2:25 pm
by NleahciM
Philba wrote:
SmileyMicros wrote:I am trying to use the Silabs CP2102 library part with Eagle and the MLF28 pads cause a DRC clearance violation with the clearance set at 8 mils as per the BatchPCB requirements. Does this mean that this part cannot be used as is? Should I edit the part to make the pads smaller or does the 8 mil rule only apply to routing?

Smiley
same problem as here http://www.sparkfun.com/cgi-bin/phpbb/v ... php?t=1832

edit the part and change the pad width to .29 to get the interpad gap to be > 8 mil.

It would be good if GP would just relax the min gap to .2 mm which is just a tad under 8mil so we can all use the datasheet recommended pad size.
Yeah - I'm hoping that batchpcb will start turning out enough boards that they can do some finer boards - maybe 4mil or smaller. 8mil doesn't give you very much to work with when you're using .5mm pitch parts...

Re: Eagle Silabs CP2102 library part DRC violation

Posted: Tue Nov 15, 2005 10:13 am
by spamiam
SmileyMicros wrote:I am trying to use the Silabs CP2102 library part with Eagle and the MLF28 pads cause a DRC clearance violation with the clearance set at 8 mils as per the BatchPCB requirements. Does this mean that this part cannot be used as is? Should I edit the part to make the pads smaller or does the 8 mil rule only apply to routing?

Smiley

Re: Eagle Silabs CP2102 library part DRC violation

Posted: Tue Nov 15, 2005 10:19 am
by spamiam
spamiam wrote:
SmileyMicros wrote:I am trying to use the Silabs CP2102 library part with Eagle and the MLF28 pads cause a DRC clearance violation with the clearance set at 8 mils as per the BatchPCB requirements. Does this mean that this part cannot be used as is? Should I edit the part to make the pads smaller or does the 8 mil rule only apply to routing?

Smiley

Well, that did not work. It lost my message on it somehow.

Anyway, waht I said, in brief, was that it sometimes helps to align the device to the grid, if it is not already aligned.

Then it sometimes helps to have the grid spacing set to the narrowest pad spacing, or a fraction thereof. It is that little job the trace makes as it enters the pad that I some times see as the cause of a DRC error. Other times it simply complains about the pad-to-pad spacing even when it SHOULD have been OK. In that circumstance, I found that realigning the devices helped.

Personally I set the grid to either 8mil or 10mil depending on the limits of the PCB fabricator.

I suppose 4 and 5 mil spacings would work well too.

I wonder what the script is to have all devices re-aligned to the grid.

I will start a new thread for that question.

-Tony

Posted: Tue Nov 15, 2005 3:00 pm
by Philba
I bet you used the autorouter. Friends do not let friends autoroute...

Yeah, its tricky to get right. I manually route because the eagle autorouter (like most others) totally sucks, blows and bites. Other than that, it's ok though... You should start your routing from the pads of the 2102 (as opposed to routing to them). select a .5mm grid and 45 deg wire bend when routing.

Note that the routing grid has nothing to do with the min spacing requirements of the PCB house. Getting your pads aligned with the routing grid will help somewhat but as I said in a previous post, I don't thinks it's completely possible. You can sort of align the chip by first doing it in the x direction and then the y. select a .5 mm grid and a .1 mm alternate. Then align in the X dimention by grabbing on the vertical pads in the very center while holding down the alt key. Slide it left or right until its .5 mm aligned. Then do the same with a horizontal pad for the y dim (up/down). The vertical pads won't have their center aligned but that's mostly ok.

Posted: Tue Nov 15, 2005 3:42 pm
by spamiam
Philba wrote:I bet you used the autorouter. Friends do not let friends autoroute...

Yeah, its tricky to get right. I manually route because the eagle autorouter (like most others) totally sucks, blows and bites. Other than that, it's ok though...

Note that the routing grid has nothing to do with the min spacing requirements of the PCB house.

Yes, I am using the autorouter. While it sucks, I suck worse! I have a really tight (to me) layout. The autorouter gives up often. I figured out how to make it keep trying.

I also fiddled the controls on trace directions, turns, etc. to get what seemed optimal for me.

With or without success of the autorouter, I looked at the areas it appeared to have the most trouble. I then tried to adjust the layout within the limits of the needs certain devices, then tried again. Once it seemed to have a decent result, I then ratsnest it and then manually route the more important or sensitive traces. Then I let the autorouter try again. I then see where MY traces seem to cause bottlenecks and also where the devices do it too. I then move devices, re-manually route and then re-autoroute.

It sounds tedious, but it is really not that bad.

All in all it seems OK. I am expecting back from the PCB house my first somewhat complicated layout. It is not nearly as tight a layout as the tough one, but I get to see how well it works.

-Tony

Posted: Tue Nov 15, 2005 5:23 pm
by Philba
I used to think hand routing was impossible but gave it a try any way. It turns out to be easier than you would think and you get A LOT more control. If you are going to do more than a couple boards, its an essential skill, IMO.

Posted: Tue Nov 15, 2005 6:54 pm
by donblake
Philba wrote:I used to think hand routing was impossible but gave it a try any way. It turns out to be easier than you would think and you get A LOT more control. If you are going to do more than a couple boards, its an essential skill, IMO.
I use "selective autorouting". I use EAGLE and autoroute one net at a time starting with Vcc then GND. I'll let the autorouter make a first attempt and then "fix" the routing manually.

Don

Posted: Tue Nov 15, 2005 7:26 pm
by spamiam
[quote="donblake]I use "selective autorouting". I use EAGLE and autoroute one net at a time starting with Vcc then GND. I'll let the autorouter make a first attempt and then "fix" the routing manually.

Don[/quote]

How do you get it to autoroute just one net at a time? That is what I would really like to do.

I would also love to be able to avoid ripping up all the traces at once. I know I can draw a box around the stuff to ripup, but I would rather preserve certain nets, and not an area of the board.

-Tony

Posted: Wed Nov 16, 2005 6:31 am
by donblake
spamiam wrote:How do you get it to autoroute just one net at a time? That is what I would really like to do.

I would also love to be able to avoid ripping up all the traces at once.
To route one net (e.g., vcc), enter the following command line:
auto vcc;
To ripup a single net:
ripup vcc;
Don

Posted: Fri Nov 18, 2005 7:39 am
by SmileyMicros
I hand route most of my boards. I actually enjoy hand routing, it seems a bit like knitting or something, anyway it is relaxing for me.

I remade the part using slightly smaller pads and it passes DRC.

Thanks for all the suggestions.
Smiley

Posted: Fri Nov 18, 2005 8:42 am
by spamiam
SmileyMicros wrote: I remade the part using slightly smaller pads and it passes DRC.Smiley
Can you tell what about the smaller pads made it pass? Was it the clearance between pads that it complained about? Was there really too little clearance for SParkfun to fabricate the board, or was it just EAGLE complaining about a figment if its imagination?

I have had this with really tight spacing on some of the super small SMT devices. I tried changing the tolerances in EAGLE without success. THen the problem went away after I repositioned the device ( and rotated it).

Go figure.

-Tony

Posted: Fri Nov 18, 2005 10:24 am
by SmileyMicros
Someone above said you can fix this by changing the grid size which sounds like what you did. The problem is that the pads are just ever so slightly too large, so I set them slightly smalller and it worked okay. I don't know how to reset Eagle so that it would pass the original and I don't know if the SparkFun DRC will allow something to pass if it is only slightly off.

Sorry,
Smiley